Tips & Tricks 2022
Until now, locking parts against processing was only possible for externally referenced parts. As of HiCAD 2023, this is now also supported for non-referenced and internally referenced parts. Locking against processing can be useful, for example, to protect an adjacent structure from unintentional processing.
This extension means that the functions for locking parts against processing are now available in a separate menu and not in the Referencing functions menu as before. You can access the function via the context menu for parts and there via the entry Lock against processing.
Up to now, when importing LogiKal items into HiCAD, the fixed setting Project name + Position was always used as the name of the top assembly, both separated by commas and with the character # in front of the number of the LogiKal item (e.g. Rounded glass, #001).
As of HiCAD 2023, only the item, the project name or the short description can be used as the name of the assembly. The Fitting options dialogue window has been extended accordingly.
- The setting for the level of detail and for the name of the top assembly Detail are defined once when importing a LogiKal item. HiCAD remembers this setting for the built-in LogiKal item. A subsequent change is not possible.
- When updating a LogiKal item imported into HiCAD, the name is also updated according to the selected name setting.
- LogiKal items imported into a model drawing with a version before HiCAD 2023 do not have a name setting. Here, the setting Project name + Position is used as the name of the assembly as before (before HiCAD 2023).
The screen display can now also be moved by holding down the right mouse button and dragging the display to the desired position. This corresponds to the behaviour of the CTRL + middle mouse button combination. If the right mouse button is simply pressed, the 3-D view context menu will be called instead.
During drawing derivation, there is often a desire to display everything on one sheet if possible. Sometimes it is also desired that sectional views, developments or axonometries should have different scales than the main view. Additionally, there are situations where the customer wants a certain drawing frame to be filled with views at an optimal scale. For example, a drawing frame DIN A2 should be used and the scale of the views should be adjusted accordingly. However, if the scale falls below 1:10, another drawing frame should be used.
This cannot be configured in the options of the drawing derivation. As of HiCAD 2023 (V. 2800) the new function Frame/scale list is the ideal solution.
Similarly to the dimensioning rules, this function can be used to define separately for each purpose, for example for assemblies, I-profiles, sheets, etc., which drawing frames combines with which scales should be used. This also significantly increases performance when creating drawings, as HiCAD does not have to search through all drawing frames and scales.
Example of a frame/scale list for sheet metal parts
A detailed example can be found here.
As of HiCAD 2023, when creating detail views, you can specify whether the detail view should be associative to the initial view or not. For this purpose, the New detail view and Change detail view dialogue windows have been extended accordingly.
Associativity to the initial view means that the detail view inherits certain changes from the initial view. These are:
- cut-outs (including the creation and deletion of cut-outs),
- the section path (if the initial view is a sectional view) and
- hatchings of cut and cut-out surfaces.
Please note the following instructions if the checkbox is active (ISD default setting).
- Associativity must be set when defining the detail view. It cannot be set subsequently.
- Cut-outs and section paths that are inherited, i.e. originate from the initial view, cannot be edited in an associative detail view. This is only possible in the initial view. However, the detail view can also have its own cut-outs, which can then of course also be edited in the view.
- An associative detail view cannot change its initial view. Marking the detail outline is possible only in this specific initial view.
- When deleting the initial view, the associativity of the detail view is lost. However, the detail view itself does not change.
- The associativity of a detail view can be removed with the Change detail view function. This does not change the detail view, it just no longer follows the changes of its initial view. Cut-outs ans section paths originally "inherited" from the initial view become the detail view's "own" cut-outs and section paths.
The figure shows a section view A-A with an associative detail view Z derived from it (1). Subsequently, a cut-out has been inserted into the sectional view (2). This cut-out is then transferred to the detail view after updating (3).
Existing detail views from older drawings (before HiCAD 2023) are non-associative and cannot be set to associative.
If parts are inserted into the model drawing where it is necessary to specify a fitting point on the part in order to place the part in the drawing, HiCAD will display an enlarged preview of the part in order to determine this point. This happens with most functions under Drawing > Insert Part.
The setting from the configuration management under System settings > Visualisation > Views > Insertion view is used as the display type for the preview (insertion view).
When inserting large assemblies, it can be useful for performance reasons to select the display type Shaded with edges. This will avoid time-consuming Hidden Line calculations.
The Hatching in Sectional View and Cut-Out function allows you to define an individual hatching for each part and view for those section surfaces that result from sections, cut-outs or detail areas. A distinction is made between "normal" hatchings and insulation hatchings.
Unlike "normal" hatching, insulation hatching is subject to special rules and requirements. The properties for insulation hatchings can therefore be defined in a separate area of the dialogue window.
Here you select the axis for the orientation of the hatching and determine the height and the horizontal scaling factor. If you want this information to be determined automatically, activate the respective checkbox next to the input field.
In addition, by activating the Hatching lines start at axis checkbox, you can specify that the insulation hatching should start exactly at the selected axis.
(1) Automatic determination, (2) Freely selected height and scaling factor, (3) Selection of the axis orientation, (4) Hatching lines start at the selected axis
In the Staircase Configurator, it is now possible to specify for intermediate platforms whether the length of the platform is to be calculated by the number of steps or by entering a value. The checkbox Calculate length by number of steps is available for this purpose. If the checkbox is active (default setting), the length is automatically calculated and displayed after entering the number of steps. This value cannot be edited. If the checkbox is not active, you can determine the length by entering a value.
When using the AutoPlace parts on guidelines function, a consistent flow at the corners of the guideline is important, especially when placing knees, because the flow direction affects the insertion direction.
Accordingly, this function checks whether the flow is consistent. If this is not the case, the function was previously aborted with a corresponding message and the corresponding point was marked with an arrow.
As of HiCAD 2022 SP2, you have the option to have the flow direction corrected automatically in such cases. The following message is displayed for this purpose:
If you select Yes, HiCAD automatically reassigns the flow, i.e. overwrites it. The input dialogue then starts again from the beginning.
If you select No, the function is terminated and the position where the inconsistency exists is marked with an arrow as before.
If necessary, you can then correct the flow yourself using the Edit flow function.
Intersections of sheets does not have to be perpendicular to the surface, it can also be carried out for lasers that cut at an angle.
You can change this setting later using the feature entry Perpendicular to surface Yes/No.
Intersection parallel to the collision parts (1), Perpendicular to surface (2)
In previous HiCAD versions, it could happen that dimension base points on standard parts were lost if, for example, the representation was changed from exact to simple or another standard part type (e.g. screw of another standard) was changed.
For this reason, the Standard part point option is available as of HiCAD 2022. This point option provides the origin of the part coordinate system of standard parts, which remains stable even when standard parts are exchanged.
The point option cannot be activated via the point option menu. Instead, the following activation options are available:
- If a dimensioning or annotation function is active, the point option can be selected via the Autopilot, provided it is active in the Autopilot Settings toolbar.
- In other functions, the point option can be used as follows:
- Move the cursor over the corresponding standard part.
- Activate the Point options menu.
- Select the point option Input via keyboard and enter NT. Then the point on the part under your cursor will be determined.
Previously, it was possible to move from one part within the part structure to the next higher and thus higher-ranking part by holding down the left mouse button and then pressing the right mouse button during Part selection in the drawing. As of HiCAD 2022 SP1 this also applies vice versa.
If you press the middle mouse button instead of the right mouse button while holding the left mouse button, you will return to the previously marked element in the part structure.
The new Shaded, without highlighted edges function provides another representation mode for views. This function shades the parts of the active view and displays all visible edges, with the exception of highlighted edges. Highlighted edges are theoretical edges that occur in places where there is no clear edge due to a rounding.
This display mode can be useful for improving the performance while working on large drawings in the model view.
(1) Shaded with edges, (2) Shaded, without highlighted edges, (3) Shaded without edges
You can find these functions
- in the context menu for views,
- in the transparent toolbar and
- under Representation in the View ribbon.
The surface colour used by HiCAD when inserting standard parts can be influenced by various settings in the catalogue tables as well as in the settings of the Configuration Editor. In detail, these are:
- the System settings > System colours table,
- the Materials > Appendix > Bolt strength classes table (for bolts),
- the Materials > Appendix > Strength classes nuts table (for nuts),
- the parameter System settings -> Visualisation -> 3-D -> Take default surface colour from Materials catalogue? in the Configuration Editor and
- the tables in the Materials catalogue.
A description that clarifies the relationship between the surface colour of standard parts and the above points can be found in the online help of the catalogue editor.
When sketching polylines, circles, arcs and ellipses, the corresponding HCM constraints are generated automatically (ISD default setting). The individual elements of the polyline are then automatically linked to each other by corresponding dimensional and positional constraints. You can activate / deactivate the automatism directly in the dialogue window of the corresponding sketch function.
While drawing sketch entities, the automatism can also be switched off for individual elements by simultaneously holding down the SHIFT key.
If the automatic setting of HCM constraints is to be switched off in principle, then you must deactivate the Create checkbox in the HCM settings at Sketch > HCM > Tools.
If you want to change the centre of a detail view of a cuboid or sphere, proceed as follows:
Activate the corresponding view and select the Change detail view function:
- For a detail view of a sphere, then select the centre point in the detail view and determine the new centre point in the original view.
- For a detail view of a cuboid, open the context menu with a right-click and select the function Move (1). You can then select the centre point in the detail view (2) and then redetermine it in the original view (3).
With cat_item_id a new 3-D function is available in the feature area. The function searches a table in the catalogue according to any criteria and returns - in contrast to the item_id function - not the row index but the Data record ID of the first item found as the result.
The first parameter is the internal name of the table to be searched in the catalogue. You get this by right-clicking the desired table in the Catalogue Editor and selecting the entry Change alias name in the context menu. The internal name of the table is then displayed in the Entry field in the dialogue box that appears. You can then close this dialogue by clicking on the Cancel button.
As an example, consider the table displayed.
In order to be able to process catalogues, you need to define unique sorting criteria for all record tables. Use the Sort values function.
The Sort values function is only available when you have opened a table and clicked once in one of the table rows. Otherwise the function is greyed out
If you want to draw an arc at the end of a line when drawing a polyline, you can - as an alternative to the Arc function in the context menu - simply select the end point of the line again (1). Then you can specify the radius (2) and, after confirming it, the opening angle of the arc (3). If the Last line option has been activated, you can then continue drawing tangentially.
The only reliable criterion when processing point clouds is the Z direction of the world coordinate system. Therefore, in most cases, a processing plane is required when constructing a point cloud, which fits the object as well as possible, but does not have an angle - even if the point cloud itself has an angle, e.g. due to inaccuracies.
To create such processing planes, the function Plane from points has been extended. In the Parallel and Orthogonal mode, you can now select either a plane or a direction. The dialogue window has been extended accordingly:
With this extended window, planes for the following use cases can now be realized as follows:
- Mode: Parallel, Plane: XZ-plane or
- Mode: Orthogonal, Plane: Z-axis
Let us assume that you want to attach further elements at the points (1), (2), and (3). The World CS is active.
Then you will select the processing planes as follows:
(1) Mode: Parallel, Plane: XZ-plane
(2) Mode: Parallel, Direction: Z-axis
(3) Mode: Orthogonal, Direction: Z-axis
Analogously to assembly points, isolated points can now also be shown/hidden in views (as of HiCAD 2022 SP1). The Show/Hide elements in view function has been extended accordingly.
Isolated points also include named points, symbol points and fitting points.
Please note that isolated points can be hidden globally by means of the Drawing > Others > Visual... function. If you have hidden isolated points in this way, they cannot be shown again with the Show/Hide elements in view function.
The function only affects the currently active view. Multiple selection of views is not possible.
For assembly points and isolated points, hiding always affects only the existing points. This means that if further isolated points or assembly points are created, these will be visible. You must first recalculate the view in which the isolated points and assembly points are already set to Hide. To do this, use the functions found under Recalculate views in the context menu of the Redraw function.
New in the Civil Engineering functions docking window at Steel Engineering > General is the Clamping plate function (as of HiCAD 2022). Clamping plates are used when parts are not to be screwed or welded.
The following connections are possible:
- One plate between two beams
The clamping plates are bolted to the plate.
- One beam and one plate
The clamping plates are bolted to the plate.
- Two beams
The clamping plates are bolted to the second beam.
(A) Plate between 2 beams, the plate is drilled; (B) Beam and plate, the plate is drilled; (C) 2 beams, the 2nd beam is drilled
For 3-D sketches, the checkbox Do not leave drawing plane is also available in the
- Angle+Distance grid,
- XY - grid and
modes (as of HiCAD 2022 SP1). Activating the checkbox causes selected points outside of the current drawing plane to be projected onto this plane and thus to be drawn in a plane.
For the On axes mode, the checkbox Do not leave axis is available, working in the same way.
The start point of the line is point (1). Point (2) is selected as the following point. If the checkbox is inactive, (2) will be the determined point. If the checkbox is active, point (3) will automatically be determined.
In HiCAD 2021 SP1, the sketching tool for planar sketches and 3-D sketches has been modernised and combined into one function. Many functions that could previously be called separately have been integrated into the new sketching tool. This applies, among other things, to the former function Tangent to edge point .
For example, if you want to draw a tangent to the end of an arc, you proceed as follows from HiCAD 2021 SP1 on:
Start a new polyline by calling the Draw polyline function (or press the middle mouse button to interrupt the currently drawn polyline). Select the end of the arc where the tangent is to start as the start point of the new line. Activate the Angle + Distance grid mode in the dialogue window and the Last line option under Angle reference. Now you can simply draw the tangent with 0° (or 180°) at the end of the arc.
Similarly, it is also possible to start a tangent from any point on the arc. To do this, the point option Z must be deactivated in the Autopilot settings.
Views can also be moved directly with the mouse using Drag&Drop. To do this, move the cursor on the view frame, press and hold down the and move the cursor to the desired position. The internal distance and angle grid for moving individual views can be increased or decreased with the + and - keys.
If views are to be locked against moving by Drag & Drop, this can be achieved by pressing the D key. After pressing the key, views are locked against moving by Drag & Drop during the current HiCAD session. In this state, clicking with the left mouse button on the view frame while holding down the mouse button causes the Rectangular zoom window function to be called up. Pressing the D key again cancels this
Please note the following when using LogiKal:
Server installations of LogiKal do not support UNC paths. In this case, a mapped drive must be specified as the path to LogiKal in the Windows Registry or in the HiCAD settings.
The dialogue of the Show/Hide elements in view function has changed (as of HiCAD 2022). The window has been tightened and, instead of checkboxes, the settings can now be selected via different selection boxes.
Hiding edges via the limiting angle is no longer available.
As of HiCAD 2022, you use the new Show/Hide edges function to show/hide any edges of the drawing. This function allows you to show or hide any edges of your drawing in the active view or in all selected views. The settings have an effect on the following representations:
- Glass Model,
- HiddenLine dashed and
- Shaded with Hidden Line.
If the desired edges are to be shown/hidden in multiple views, select the corresponding views in the ICN before calling the function.
After calling the function, the dialogue window Show/Hide edges will be displayed.
Then, select the desired edges in the drawing. Each selected edge will be included in the list in the dialogue window and visualised in colour in the drawing. If an edge that is contained in the list is selected again, it will be removed from the list. In multi-part sheets, when an edge is selected, the congruent edges of the flange and bend zone are also automatically selected.
When clicking on an entry in the list, the corresponding edge in the drawing will be highlighted in colour.
If multiple views were selected when the function was called, it is possible to specify for each edge contained in the list whether the edge is to be hidden only in the active view or in all selected views.
You can hide the edges presented in the list by clicking OK.
When you call the function again, all hidden edges will be listed in the dialogue window. To show the edges again, simply delete the corresponding list entry.
Tips & Tricks 2021
In the ICN, place the mouse pointer on the part you want to move. Hold down the left mouse button and drag the part to the new position within the part structure.
While dragging, you can also use the scroll wheel of the mouse for quick navigation. Then, move the mouse pointer onto the part to which you want the selection (together with subordinate parts) to be assigned and release the mouse button.
In acute corners, the outer contour cannot be milled exactly with the standard milling cutter. In practice, a cutter with a smaller diameter is used here. In the development calculation, paths for the treatment of acute corners can optionally be generated on a separate layer.
To display the path, check the option Paths for acute inner corners. Then enter the angle up to which the path is to be generated. You can also set the path length, layer, color and line type.
The path does not lie exactly on the outer contour (distance of 0.01 mm) to prevent it from disappearing during export.
(1) Sheet metal part, (2) Development, (3) Enlargement of the path for the acute inner corners with a path length of 0.3
HiCAD offers the possibility to save the ICN display together with the drawing. In this way, the HELiOS attributes are also displayed in the part structure of the HiCAD Viewer. It is either possible to temporarily perform the setting during the current HiCAD session or set it as a default setting in the Configuration Editor.
Sometimes generating the ICN can lead to considerable waiting times. As of HiCAD 2022, if the Save ICN display with drawing status is active, the new message
Save drawing (generate ICN designations for Viewer)
will be displayed in the user guidance (info toolbar) during the saving process. This enables you to see that the status is active and could possibly be the cause of the waiting time.
The Smart dimensioning function of the Sketch HCM can also be used to set arc dimensions. To do this, first select the arc (1) after calling the function. The radius dimension of the arc (2) is now attached to the cursor. Then simply select one of the dimension base points (3) and drop the dimension (4).
Previously, it was not possible to incorporate assemblies and parts with subordinate parts from the Purchased/Factory standard parts catalogue. As of HiCAD 2022, this is now supported.
This means that, in addition to assemblies, for example, Sheet Metal parts stored in the Purchased/Factory standard parts catalogue can now be incorporated into the drawing using the Purchased/Factory standard parts function. However, it should be noted that these Sheet Metal parts are combined into a solid during installation. This means that the installed part will no longer be considered a Sheet Metal part from the HiCAD point of view!
When saving your own factory standard parts to the Purchased/Factory standard parts catalogue, please note the following:
- If you work with your own tables, make sure that these tables are assigned to the Purchased/Factory standard part category. You assign this when creating the table.
- The fitting position must be defined in the parts stored in the catalogue (.KRA files). To do this, you define a Fitting CS. This consists of 3 special points which are automatically assigned the point designations #1 for the origin, #2 for the X-direction and #3 for the Z-direction.
- To save the parts, use the Reference part, Save, Detail drawing function.
If the By assemblies numbering mode is selected during the itemisation, then the identical part search and the assignment of item numbers will take place within the assembly. It may happen that two different parts from two different assemblies are given the same item number.
Previously, when creating a workshop drawing, only one of the two parts was output and detailed in cases like this. As of HiCAD 2022, the numbering mode of the itemisation will be taken into account during drawing derivation. This means that the parts will no longer be compared only according to the item numbers but also according to the level of the part structure.
The drawing illustrated here consists of two assemblies, each including a composite panel, one of which contains bores. If this drawing is itemised by assemblies, both composite panels - although different - will receive the same item number.
Now the drawing is created via the settings shown at the top right. The following illustration shows the drawing created with HiCAD 2022 on the left and the drawing created with HiCAD 2021 on the right.
With HiCAD 2022, the internal data format of annotations has changed. During the creation of new annotations (also in drawing derivations and sheet developments), the new format is always used. Visually, there are no differences to the "old" format. When loading a drawing that contains annotations created before HiCAD 2022, the following message appears:
If you click on Yes, the previous annotation tags will automatically be converted to the new format. A message is then displayed, indicating whether or not all annotation tags could be converted, e.g.
In the ISD Configuration Editor, under Compatibility > Annotations > Part annotation, 3-D, you can preset how to proceed when constructions with "old" annotation tags are loaded and whether a message should be output after a conversion.
The conversion of old annotation tags can also be done automatically by setting the Convert part annotations of the drawing when loading? parameter to Yes, without query.
From HiCAD 2022 onwards, you have the possibility to upload files directly from HiCAD if you are using the ISD File Centre for data exchange with the ISD Support. For this purpose, the new Load file into ISD File Centre function can be found in the Help menu.
The post connection for the substructure can now be determined separately for start, intermediate and end posts and corner posts.
Start and end posts can also be determined individually, i.e. independently of the intermediate posts. To do this, you must activate the corresponding checkbox at the top of the dialogue window.
Railing with lateral connection of the start, corner and intermediate posts and connection from bottom for the end post
If several point cloud parts have a missing reference when loading a model drawing, it is often the same reference. In this case, the reference does not have to be selected again for each part, but all parts with identical reference are updated accordingly. This means that it is sufficient to select the new reference for one of these parts.
New in the Drawing attributes dialogue window is the checkbox Itemised source model. This checkbox (Attribute #PMOD) determines whether a model drawing is an itemised source model or not. An itemised source model is a model drawing in which itemisation is allowed. The ISD default setting is that new model drawings are always itemised source models, i.e. the checkbox is active by default.
If you are not able to find the Itemised source model checkbox in your Drawing attributes window, e.g. after installing an update, you can insert it as follows:
- Close HiCAD.
- Open the brw_szene.hdx file, that is located in the HiCAD SYS directory, with an editor.
- There, insert the following line:
- Save the file.
- After you restart HiCAD, the checkbox will be available.
The Design Checker can be used to check sheet metal parts for collisions between flanges or bend zones during a development or bending simulation.
As of SP1, it is also possible to group the result list by item numbers in the function Part statistics .
However, grouping by item numbers is only supported if the itemisation was done in the By model drawings mode. Otherwise the option Item number is greyed out.
In HiCAD version 2601.1, the use of Nvidia graphics cards can result in shortened axonometric views being displayed incorrectly. This is due to the fact that the graphics card driver is outdated. This effect does not occur with an up-to-date graphics card driver.
We recommend updating to a current graphics card driver, even if the old graphics card driver supports the required OpenGL version 4.3!
If you encounter any kind of display problems, please check if your graphics card driver is up-to-date first. If it is not, update to the current driver.
Divide along direction (3-D Standard > Process > Trim > Divide along direction)
Divide along direction (Steel Engineering > Lengthen > Divide > ...)
have been revised. As of HiCAD 2021 SP1 dividing can now also be done by selecting points. The division points do not have to be on the part.
The Update import, via 3-D interface function has been extended in SP1:
After the update, an evaluation of the update is displayed with the following information:
- parts in the previous import,
newly imported parts and
- unambiguously assigned parts among them.
This dialogue is used to illustrate to what extent it was possible to transfer the attributes from the old parts to the new ones and whether there were changes in the number of parts.
In the following cases, a warning message is issued before the update:
- In HiCAD, parts of the old import have been changed or deleted.
- In HiCAD, new parts have been inserted into the assembly of the old import.
All corresponding parts are listed in the dialogue window. Only parts that are visible in the ICN are taken into account.
The icons on the left of the dialogue window can be used to vary the display. The log can also be exported as a CSV file via the icon at the top of the window.
If the dialogue window is closed with OK, the update is started. Thereby the parts and changes in the list will be lost
As with Sheet Metal parts, the calculation of the length and width of Steel Engineering beams now also takes into account whether a processing direction is assigned to the plate.
The processing direction also affects the position of the plate in the workshop drawing.
2-D data is generally not exported via the 3-D PDF interface. To output 2-D data in PDF format, you must use the Print function. For this, you need an appropriate printer driver, e.g. Microsoft Print to PDF, Adobe PDF or similar.
If you have the ISD Fileprinter PS, you can also use Ghostscript, for example. In this case, you must activate the Postprocessing checkbox in the ISD Fileprinter PS dialogue window and enter the corresponding command for the conversion in the comment line, e.g. for Ghostscript 9.54
C:\Program Files\gs\gs9.54.0\bin\gswin64 -dNOPAUSE -dBATCH -dPDFA -sDEVICE="pdfwrite" -sOutputFile="<FilePath><FileName>.pdf" <CurrentFile>
New in the Drawing attributes dialogue window is the checkbox Itemised source model. This checkbox (Attribute #PMOD) determines whether a model drawing is an itemised source model or not. An itemised source model is a model drawing in which itemisation is allowed. The ISD default setting is that new model drawings are always itemised source models, i.e. the checkbox is active by default.
Model drawings that are not itemised source models cannot be edited with the Automatic itemisation functions. This also applies to deleting any existing item numbers. If an Automatic itemisation function is called, the following message appears:
Deactivating the checkbox is useful, for example, if you want to disable itemisation in model drawings when passing them on to third parties.
If a model drawing with item numbers subsequently becomes an itemised source model by activating the checkbox, all existing item numbers become invalid.
When working with the Drawing Management, the checkbox Itemised source model is not available. Use the ITEMISATIONMODEL attribute there for this purpose.
When sketching lines, additional options are available for 3-D sketches when determining points via the Autopilot:
is displayed if the X-coordinate of the current cursor position is identical with the X-coordinate of another point in the active 3-D sketch.
is displayed if the Y-coordinate of the current cursor position is identical with the Y-coordinate of another point of the active 3-D sketch.
is displayed if both the X- and Y-coordinates of the current cursor position are identical to the X- or Y -oordinate of another point in the active 3-D sketch.
Together with the display of the point option, a dashed auxiliary line is also displayed on the point with identical X- or Y-coordinate. All points of the active sketch as well as the origin (zero point) of the sketch are taken into account.
However, the options X, Y and XY are only available on the Autopilot if these points are in the current drawing plane.
The 3-D sketch shown at the top left is to be created - consisting of 3 polylines. For the first two polylines, the point options X and Y can be used for the dashed lines (A). This is not immediately possible with the third polyline (B). Here the drawing plane must first be changed (C).
3-D parts/assemblies that you insert into the current model drawing using the function 3-D Import will be marked in the ICN with the symbol.
With the new function Update import you can replace these parts/assemblies with other imported files. You can access the function by right-clicking on the marking, or via the context menu for parts.
The prerequisite for the update is that the top assembly of the first import still exists and the part on which the update is called is below this assembly or is itself this assembly. The assembly of the old import is completely exchanged for the newly imported one. This means in particular that parts that were added to the assembly after the import are lost during the update.
You can access the function
by right-clicking on the marking of an imported part in the ICN or
by right-clicking on an imported part in the ICN or in the drawing. In this case the context menu for 3D parts is activated. There you will find the function in the Others sub-menu.
For further information click here.
It occasionally happens in parameterized model drawings that the value of a variable must be selected from a list depending on the value of another variable.
An example of this is an element for a facade, for which an attic with the lengths
- medium or
can be chosen. The selected variant is stored in the variable type - 1 stands for "short", 2 for "medium", 3 for "long". If now the value of the variable length is to be set dependent on type, you can set the variable length with the following formula:
If type=1, length has the value 100; type=2 leads to length=250 and type=3 results in length=600. Of course, you are not restricted to 3 different variables, but can use any number.
Note on the keyword LAYER of the conversion file HCADACAD.DAT:
The Layer assignment based on part structure option can only be applied to 2-D parts whose name does not exceed 8 characters.
Purchased/factory standard parts and moulding tools are also placed in the model drawing via the Fitting CS of the corresponding KRA file or via three isolated and named points defined in the KRA file (Point 1 for the origin, Point 2 for the X-direction, Point 3 for the Y-direction). If neither these points nor a Fitting CS are defined, the following message appears from HiCAD 2021 onwards:
HiCAD relies on the operating system of the workstation for file access. Thus UNC paths or mapped drive letters in the filegrup.dat should work exactly when these can also be accessed via the file explorer without authentication questions being asked. Special log specifications (as prefix or path specifications) are not supported.
If directories are accessed from more than one workstation, no local path should be entered in the filegrup.dat at C (for the "Szenen" directory), but the full UNC path as shown below:
For detailed information about filegrup.dat click here.
As of HiCAD 2021 the active view is now represented in the model drawing by a coloured, wider view frame.
The frame display of the active view - colour, line width and transparency of the frame - can be preset in the Configuration Editor at System settings > Visualisation > Views > Frame of active view. You determine the colour by specifying the RGB values. There you can also set whether the active view should be marked or not. The image below shows the ISD default settings.
In practice, model drawings often contain beams, e.g. purchased parts, which are ordered for the production with a fixed length. These beams should not appear in the bar list or must be shown separately.
In HiCAD 2021 this can now be regulated via the attribute Fixed length (%FIXLEN), which must be assigned to the corresponding beams. If this attribute has the value 0 or is not set at all, the fixed length is not taken into account in the bar list. If the value is 1, then these beams are listed separately in the bar list.
By default, the attribute is not set, i.e. it is not included in the attribute masks. If you want to use this attribute, you must manually extend the attribute mask for beams by adding the files
- BRW_3DTeil_Profil.HDX (part attributes for beams) or
- BRW_3DTeil_Profil_H.HDX (part attributes for beams that are assembly main parts)
accordingly. You can find an example here.
HiCAD offers a very extensive range of functions. Therefore, it can happen that one is looking for a certain function but does not know exactly on which Ribbon the function can be found. In such cases, the new Function search docking window can help (as of HiCAD 2021).
If you enter a search term in the docking window, HiCAD lists all functions whose name contains the specified search term. The search is carried out in all ribbon bars as well as in the functions of the docking window Civil Engineering functions.
If you right-click on a function, the function can either be called up directly (Execute), or you can open the Help for this function, or Copy the function path.
You use the program CatalogueUpdate.exe in the HiCAD EXE directory to update catalogues. This program is normally started automatically, e.g. when HiCAD is updated. It can also be started manually.
For automatic updates the source is preset.
If the program is started manually, then the source is to be selected as follows:
- for a HiCAD Update:
on the DVD or in the ISO file of the update.
- in case of a HiCAD Patch:
on the DVD or in the ISO file of the patch.
For foreign language installations, replace en-us with the corresponding language abbreviations, i.e. de-de (German) fr-fr (French), it-it (Italian), pl-pl (Polish
In the Internal/external thread function , thread runouts are now also possible (as of HiCAD 2020 SP2). The following options are available for runout length determination :
- Value, as part of thread length
The runout has the length specified in the Value field. The specified thread length is shortened accordingly.
- Value, in addition to thread length
This is only possible with the length options Fixed length and To point. The specified value determines the length of the runout, the thread length does not change. If the sum of thread length and runout length is greater than the possible full thread length, the runout is automatically shortened.
- Pitch factor, as part of thread length
The specified factor is multiplied by the thread pitch. The result is the runout length. The specified thread length is shortened accordingly.
- Pitch factor, in addition to thread length
This is only possible with the length options Fixed length and To point. The specified factor is multiplied by the thread pitch. The result is the runout length, the thread length does not change. If the sum of thread length and runout length is greater than the possible full thread length, the runout is automatically shortened.
(1) Thread DIN 13 -M50x1.5, (2) Runout length 20, (3) Runout factor 8, (4) Internal thread DIN 40x1.5 with runout
HiCAD 2020 features a new movement type called AutoDirection on the Exploded view Ribbon tab.
This function allows you to define displacements with automatic direction in the Exploded view mode. As with the displacement, several parts are linearly displaced simultaneously. In contrast, these parts are not moved with the same distance, but are distributed along the selected direction relative to a certain part (the so-called fixed part). This makes it possible to move several parts simultaneously in positive and negative direction in one step - depending on the position of the parts in relation to the selected fixed part.
In the image below, take a look at the initial drawing shown on the left. We want to achieve that the selected parts (1) - highlighted blue in the figure - are moved on both sides of the fixed part (2) in one step, depending on their position relative to part (2). The desired result is shown in the figure below. This can be achieved with the AutoDirection function.
Tips & Tricks 2020
The previous functions Detail view Cuboid and Detail view Sphere have been combined to form the new function Detail view Cuboid/Sphere . You can switch between both modes in the Detail view dialogue window..
The new dialogue is much more user-friendly. For example, the cuboid and sphere are now visualized in the preview and can be drawn dynamically with the cursor.
From SP2 on it is also possible to change a Detail view Cuboid / Sphere subsequently. To do this, select the Change detail view function in the Views Ribbon or in the context menu for views. Afterwards the corresponding dialogue window is displayed.
The settings for the 3-D Import function can now be saved as favourites. To do this, click on the symbol in the dialogue window. You can find more information on favourites management in the in the Manage Favourites topic of the HiCAD Basics Help. You can specify which favourite is used as the default in the import dialogue in the Configuration Editor at Interfaces > Import.
To preset a favourite for a file format, just click on the symbol and choose the desired favourite.
When starting the import dialogue, please note that the last selected settings for the respective file format are used as default. If you have not made any changes to the settings of the favourite defined in the configuration management, the favourite settings will be used.
With the Design Variant Cross-bracing (2602) it is also possible from SP2 onwards to connect two perpendicular beams to each other with a diagonal using a cross-bracing.
The contents of various docking windows can be enlarged or downsized dynamically by zooming (as of HiCAD 2020 SP2). This is possible for the following docking windows:
- 2-D/3-D Part structure,
- HCM (2-D) und HCM (3-D),
- Part variables,
- Exploded view.
- To enlarge or downsize the contents of a single docking window, point the mouse cursor inside the window and turn the mouse wheel while holding down the CTRL key.
- To enlarge or downsize the contents of all docking windows, turn the mouse wheel while holding down the CTRL and the SHIFT key.
- The zoom of the active window can be reset by pressing the CTRL and middle mouse button simultaneously.
- To reset the zoom of all windows, press CTRL, SHIFT and the middle mouse button accordingly.
The Design Checker offers a new check for sheet metal parts called Sheet must contain exactly 1 direction symbol. This check finds all sheet metal parts with no or more than one direction symbol (as of HiCAD 2020 SP2).
The scope of delivery of the As-Built Modeler from FARO® includes a SendTo App. This can be coupled with HiCAD, so that points determined with the As-Built Modeler can be used directly in HiCAD. These points are treated as points with absolute coordinates, i.e. they have no reference to HiCAD objects.
To use points from the As-Built Modeler in HiCAD, proceed as follows:
- In addition to HiCAD you start the HiCAD Connector. To do this, execute the file HiCADPoint3DConnector.exe in the EXE directory of the HiCAD installation.
- Start the SendTo App in the As-Built Modeler by clicking on the symbol.
- Connect the SendTo App with the HiCAD Connector. For this purpose drag and drop the symbol from the SendTo toolbar onto the HiCAD Connector. If the connection was successful, the symbol changes to .
- If you now start a point selection in HiCAD and then click on Point selection in the SendTo App, the coordinates of the point selected in the AS-Built Modeler will be transmitted to HiCAD as absolute coordinates.
New Autopilot settings toolbar
Using the new toolbar, you can now control directly in the status bar which points the Autopilot offers as snap points. Switching is possible at any time - even during the execution of a function.
The currently selected autopilot settings apply to the active HiCAD session. You can define which settings should be active when restarting HiCAD in the Configuration Editor at System settings > Identification with the parameter List of point snap options.
If you click on the in the Autopilot Settings toolbar, the settings from the Configuration Editor are restored to defaults.
New Visualisation toolbar
The previous toolbar "CS display" has been extended with additional functions for fast fading in and out of objects and renamed Visualisation. With the functions of this toolbar you can switch on or off the visibility of coordinate systems, isolated points, dimensions, HCM constraints etc. with one click. In certain situations - especially with large model drawings - this can make editing easier. For example, you can hide all dimensions of a model drawing without having to call a function in the context menu or ribbon first.
When selecting attributes for annotations, you now have the option to mark frequently used attributes as favourites for a faster access. Simply click on the symbol next to the attribute name. The symbol then changes its colour to yellow . Attributes marked in this way are listed in the selection window under Favourites.
To remove an attribute from the Favourites list, simply click on the corresponding symbol - either directly in the Favourites list or in the attributes list.
Output associated assemblies
In the Configuration Editor at PDM > Management+BIM, you can (as of HiCAD 2020 SP1) define whether the associated assemblies, e.g. welded assemblies, should be determined for individual parts (beams, profiles, plates, sheets and general parts). The parameter Output associated assemblies is available for this purpose. If this parameter is set to Yes, the association is determined and assigned to the HELiOS article attribute COMPONENT_REFASSEBMLY. This can be useful for the BOM output, for example.
The COMPONENT_REFASSEMBLY attribute is assigned the item number of the first parent assembly of the part. If a part exists in several assemblies, the item numbers of the parts are separated by semicolons.
Starting with SP2, the total number of the parts in the assemblies is also determined and assigned to the COMPONENT_REFASSEMBLY attribute.
Further information on the COMPONENT_REFASSEMBLY attribute can be found here.
Please also note the new Output construction section list in drawing function introduced with SP2. This function is used to insert a construction section list into the drawings of the individual parts. This BOM shows how often a part is present in the different construction sections.
Within the Create Clipping Box or Edit Clipping Box function, you can right-click to open a context menu with further functions.
With this functions, the current clipping box can be rotated or moved. If you choose Rotate, the clipping box can be rotated around an axis by selecting the rotation circle of the respective axis with the cursor and then rotating it dynamically with the cursor.
(1) Current clipping box, (2) Selection of Z-axis as rotation axis, (3) Rotated clipping box, (4) Cropped point cloud
When generating the DXF export files for Sheet Metal blanks, the orientation of the polylines in the created DXF file will now always be always the same (i.e. always clockwise or always anticlockwise), since CAM programs require these for determining the outer/inner side when generating the milling tool paths.
As of HiCAD 2020 the orientation of closed lines can be set when exporting sheet metal developments. In the Configuration Editor at Sheet Metal > Sheet development you can set a clockwise (activate checkbox) or anticlockwise orientation (deactivate checkbox) for the inner and outer contours.
With the 3-D Import function, parts inserted into the model drawing can also be searched with the Find function in the transparent toolbar. The part filter dialogue has been extended accordingly.
All parts that you insert into the model drawing using the 3-D Import function are marked with the symbol in the ICN. If you place the cursor over the symbol, you will obtain further information on the relevant part, such as the imported file format and the HiCAD version with which the part was imported.
An API (Application Programming Interface) is a collection of definitions that allow a computer program to communicate with another program or part of a program (usually in the form of libraries).
HiCAD also provides an API based on .NET technology. This means that functions which are available in HiCAD/HELiOS can be accessed via a universal programming language. These functions are accessed via libraries. Via this programming interface HiCAD can also be controlled, extended and analyzed from other Windows applications. The API can be addressed by any modern programming language, for example C#, VB, C++, Java and others. On the basis of the API it is also possible, for example, for the Consulting department, for external employees or for partner companies to carry out HiCAD developments.
- Working with the API does not require an additional module, but requires the participation in a training course.
- After the installation of HiCAD, the online help of the API can be found in the HiCAD sub-directory docu\api.
For the import, display and editing of point clouds a license for the HiCAD Point Cloud module is required. HiCAD model drawings containing point clouds can be opened without such a license, but the point clouds will then not be displayed.
If you want to reset the HiCAD user interface, for example because ICN windows are no longer displayed or because incorrect icons or texts are displayed in the HiCAD toolbars or ribbons, use the contains the tool
tool in the HiCAD EXE directory. This tool resets the entire HiCAD user interface, i.e. all corresponding settings in the Windows Registry and in the %APPDATA% directory, to the state after a new HiCAD installation.
After starting the tool, the following dialogue window is displayed.
HiCAD should be closed before calling the tool.
You start the reset by clicking the Restore GUI delivery state button. With the functions and the current settings can be saved and reloaded at any time. The file format is hicadgui. This is also useful if you use HiCAD at different workstations, e.g. on a laptop and on a computer with two monitors. You can simply save the settings of both workstations and then load the respective settings file you need.
For further information click here.
As of HiCAD 2019 the “old” itemisation, i.e. the itemisation that was used up to HiCAD 2017, will only be available for model drawings that were already itemized with these functions. From HiCAD 2021 onwards, only the “new” itemization will be supported.
As of HiCAD 2020 SP1, you can use the Configuration Editor to define the procedure for starting the itemization in a model drawing that still uses the itemization up to HiCAD 2017. To do this, open the Configuration Editor and choose System settings > Itemisation > Switch to 'Standard itemisation used since HiCAD 2018'.
The following options are available here:
No message or query will be displayed. This means that the itemisation up to HiCAD 2017 will still be used.
A message will be displayed, informing you that the itemisation up to HiCAD 2017 will still be used. You then have the option of determining whether or not the itemization should be converted to the standard itemization. To Cancel the itemization function, use the same named option.
Here, too, the message will be displayed, informing you that the itemisation up to HiCAD 2017 will still be used. Here, however, you only have the possibility to switch to the standard itemisation with OK or to Cancel the itemization function.
The default setting is Optional.
For further information click here.
The detail drawings created with the Management+BIM module are always stored on Sheet 2 of the drawing. When printing via the HELiOS/HiCAD Spooler, all sheets are printed - depending on the setting - i.e. also sheet areas without production drawings such as Sheet 1.
By setting (Configuration editor) the Delete unused sheet areas parameter to Yes you can now specify that sheet areas without production drawings are deleted. The default setting is No.
As of HiCAD 2020 the Design Checker offers additional tests for HCM models.
When installing elements - especially for complex facades - it is often the case in practice that certain installation elements have the same options. To make it easier to select the areas to be occupied (rectangular or polygonal sketch areas) and to edit installation elements with the same parameters, HiCAD offers the possibility to work with so-called selection groups. The advantage is that you can group installation elements with the same parameters and then select or deselect all elements of this group with one click. The Selection groups area is available in the Installation elements dialogue window.
Selection groups can also be applied to Sub-structures.
In the Configuration Editor at System settings > Catalogue > Track catalogue changes you can now determine how to proceed in case of catalogue changes in HiCAD. The default setting is Do not track, that is, the catalogue data will be loaded only once when you start HiCAD. After this, HiCAD will no longer check whether newer data exist. The reason for this is that a check for up-to-dateness of catalogues in HiCAD can significantly deteriorate the performance in some situations.
As of HiCAD 2020, the new Reload function offers the option to update catalogues after applying changes to them without having to close HiCAD, and without having to put up with drops in performance due to repeated checks for up-to-dateness.
You find the new function at Settings > Catalogue.
In previous versions, dimensions were always assigned to the active part during their creation. From HiCAD 2020 onwards, you can assign the dimensions either to the active part or to the part to which the 1st dimension base point belongs. This behaviour can be determined via the Set parameters for new general dimensions function, on the System tab of the dialogue window.
The parameters of this tab can be preset via the Configuration Editor, at System settings > Annotations > Dimensioning, 3-D > Interactive dimensions > Dimension assignment. The default setting is Active part.
As of HiCAD 2020, the active pipeline is determined via the active part.
This means: If the active part belongs to a pipeline, then this pipeline is considered the active pipeline. Otherwise, no pipeline is active.
The previous functions for activating pipelines are therefore no longer available from HiCAD 2020 onwards.
Checkup and Release can now take place directly in the production drawing. In previous versions these options were greyed out if a production drawing had been loaded.
In the Sketch HCM the constraints will now (as of HiCAD 2019 SP2) take into account whether the use of external references has been activated or deactivated. An external reference exists if a HCM constraint refers to a part that does not belong to this sketch.
In existing sketches the use of external references is active by default, in order to keep the existing behaviour of these sketches. Created new sketches behave according top the settings specified in the Configuration Editor: The value chosen at System settings > Sketch HCM > Use external references determines your default value. After new installations, external references are not used by default.
If you right-click on the empty area of the HCM window of the ICN, a context menu with the options External reference: Use or ... do not use, respectively, will be displayed, which shows you the current setting for external references. After choosing this option, a dialogue window will be displayed, allowing you to choose between the settings Use and Do not use.