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Emil Rindell
Jonas Bryntesson
Henrik Andersson
2020-01-01
Emil Rindell
Jonas Bryntesson
Henrik Andersson
2020-01-01
IRONCAD has something called configurations. This means that assemblies, partners and features in the same 3D file can have different positions and visibility (suppress mode = shown or not shown). For example, configurations can be used to show a assembly in exploded mode, to show different steps for assembly instructions, to show how a solution will look in different predefined modes, different ways to solve a problem by showing and hiding different things in different configurations, or to show a sheet as it looks before and after manufacturing.
Configurations can also be used to show only a single part or subassembly, which is then depicted on the drawing. All other parts and subassemblies are then suppressed in the 3D scene. This is a viable option instead of saving the part to an external file. When unfolding a sheet (Sheet Metal Unfold), a configuration is automatically created which allows you to quickly switch between folded and unfolded mode. Configurations do not support different colors for parts or the ability to use different properties such as User Name, Part Number, Description or other Custom Properties.
Clicking on the Configurations button will open a settings window.
Displays the configuration currently active in the 3D scene. By default, the Default configuration is always active and is always available when creating a new 3D scene. The Default configuration can also not be deleted as it is system defined.
A list of the configurations available in the open 3D scene. The configurations are shown in alphabetical order and cannot be adjusted in a different order.
Creates a new configuration via a new window with options for how the configuration should work.
Allows renaming the selected configuration.
The name will appear in a new window. You can rename both active and inactive configurations.
Removes the selected configuration. NOTE! No warning will appear if you delete a configuration.
Activates/switches to the selected configuration.
Displays the settings that are active for the selected configuration. What the settings mean is described further down the page.
At the bottom is a setting that controls how configurations are handled in externally linked files. With this setting enabled, only changes made in the main configuration will work. We recommend keeping this setting disabled, as it will counteract changes made in the external files. If a change is made in an externally linked sub-assembly and you then switch to the main assembly, the changes will NOT take effect. However, the old settings in the main configuration will now take effect back down to the sub-configuration and then delete what you last did!
Click on the Create... button.
Name the configuration, perhaps Burst Mode, Min configuration, or something else that describes what the configuration handles.
Then select the options that fit this configuration.
In particular, there are three settings to choose from.
New Parts/Assemblies added within context of other configurations are suppressed in this configuration.
Straight translation: new parts and subsets added in other configurations are automatically suppressed in this configuration. Or simply explained: allows hiding parts and subsets via suppress in this configuration. Things added in other configurations are hidden.
Track suppression for Intellishapes in addition to Parts/Assemblies
Also hide features (Intellishapes such as holes, radii, etc.) in addition to parts and assemblys
Selecting this option also gives a warning that the file size may grow and regeneration times may become more frequent due to features being switched on and off when switching configurations.
Configuration stores position of Parts/Assemblies
The configuration saves the position of parts and assemblys.
Note: If the parameter table is used to control visibility (suppress), these parameters will take precedence over settings controlled via configurations.
The three most common variants of configurations and their options are as follows:
Hide some items and allow you to move other items apart.
Hide some items and allow you to move other items apart. Usually several configurations with the same setting, e.g. Mode 1, 2 etc.
Hide some items and anything added in other configurations is automatically hidden in this configuration.
Exploded configuration (for free positional movement)
Used only for 3D files where the parts are positioned with constraints. With this option selected, the anchor point is released and you can freely drag the parts around, even though they are locked together with constraints. This is the only way to disassemble locked objects, without destroying or removing the constraints.
Note: Position and projection locks will not be taken into account in this configuration, but positions will still be saved. This setting is automatically enforced down to external links. If you want to create a broken configuration, you should primarily use option number three Configuration stores position of Parts/Assemblies and not this one.
It is possible to switch the configuration for linked external files, parts or assemblys. Maybe you want to display a subset in a different predefined mode and since you have already created a configuration in its own file, you can easily access that configuration. By right-clicking on the path directly below the icon for externally linked parts or assemblys, the option to toggle the active configuration is available.
In the Scene Browser, expand the part or sub-collection by clicking on the plus sign and then right-clicking on the icon where the path to the external file is displayed. After selecting Change Configuration... this box will appear where you can switch between different modes for the linked subset or part.
Choosing which configuration an externally linked part or subset should use will not affect other instances of the same file. So you can use the same file for different projects, but use different configurations in each instance, without affecting the original.
When a sheet is spread, a new configuration is automatically created with the spread sheet. This is partly so that you can quickly switch to the spread mode without having to wait for a new regeneration of the plate, but more importantly to be able to map the spread plate on a 2D drawing. To unfold a plate, right-click on it and select Unfold. This automatically creates a configuration called Unfolded "name of plate".
When creating views in a 2D drawing, the options for active configuration are displayed via a drop-down menu just below the path to the file.
You can also select the configuration of an already deployed view in the 2D drawing. Either by selecting the view and changing the configuration in the Drawing Browser on the left side.
Or right-click on a view and select Properties.
When creating a Bill of Materials (BOM), the list of available configurations is displayed at the bottom left.
It is always a good idea to choose the Default configuration instead of No Configuration Selected, as the latter also shows suppressed objects but is always the default. The Default configuration is usually the one depicted in views and therefore the one the BOM is likely to reflect. If you have recurring problems with the chunk list showing more than it should, this is usually the reason.
A parts list does not have to reflect what is shown in the drawing views. You can specify a different configuration for the parts list than the one used to depict the views. It is also possible to change the configuration of an existing parts list afterwards. Right-click on the parts list and select Properties, then at the top there is a drop-down menu with the configurations you can choose from.
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