How to create multiple configurations within an assembly?

[JeffKwapien]

Does anyone know if Pro/e has a command (similar to Ideas "assembly configuration" option) in order to create multiple configurations of an assembly, so that each configuration has a unique set of component constraints?

I could not find something similar in Pro/e 4.0 help menu.

I simply want to create multiple assembly configurations within one assembly model, without having to learn about Mechanisms.

Thank you

[KevinBradberry]

The following thread may be helpful:

http://communities.ptc.com/message/4910#4910

Welcome to PlanetPTC.

[JeffKwapien]

Thank you for the quick reply. Unfortunately, I first read every post before deciding to send out my question. I wanted to see if I missed something in Pro/e's help menue. I think I may have a work around, which is to create multiple constraint sets, followed by creating individual drawings by activating only one constraint set at a time.

[KevinBradberry]

Is your goal to have a drawing of each assembly configuration? Is each configuration going to look different, like a set of legos that you can build in many different ways? Please give more details for what you end goal is. I'm wondering if the best option would be to have separate assemblies with a drawing for each.

[JeffKwapien]

My goal is to show multiple ways to build the same assembly, it doesn't matter whether it is in one drawing or several. I would like to be able to do this using one assembly file. The only variables are in a set of angle-mate constraints which constrain the subassemblies to eachother with multiple sets of angles. It doesn't matter whether I show multiple assembly configurations in one drawing or multiple drawings, but I wanted to have just one assembly file. I believe I can do this with multiple constraint sets, but after I created my second constraint set, by disabling my previous set, somehow, the disabled constraint set disappeared from the assembly. I'm not sure if Pro/e deletes disabled constraint sets during regeneration. Ideas software had a "Configuration" command within their "Assembly" module that would allow you to turn on/off various assembly configuration constraint sets. Is this feature also in Pro/e? Thank you.

[KevinBradberry]

I don't know of an equivalent command in Pro/E like you have described in I-DEAS.

However, I think one possible solution would be to assemble all variations of your parts into one assembly and then set up Simplified Reps to demonstrate each configuration that you want while hiding the ones that you do not want. For instance, Sim Rep 1 could have part A mated with part B. Sim Rep 2 could have part A angle aligned with part B. In this simple example the assembly file would have 2 A parts and 2 B parts.

When you create the drawing you can assign a Simplified Rep to a drawing view.

[vzak]

Hello,

if your only modification is different constraint sets, then straight forward tool will be assembly family table :

1. Create all variations of Constraint Sets for the components you want to vary. Add meaningfull names to sets, like : Position_1 / Posiyion_2 etc

2. create number of instances in assembly family table - as many as combinations that you need.

3. Add column items as Paramaters / select Component Parameters / go pick your component that have more than 1 Set - and you will have an option to choose parameter called PTC_CONSTRAINT_SET. Add them per each component.

4. In the values for this parameters, put respective sets names in each cell. Your family table is ready now.

5. enjoy

p.s. sure if you have nested structure (variations in different subassemblies) this will require creation of such family table at each level.

[Dale_Rosema]

Or if it is an assembly that can be in several different positions, you could you family tables to show the different assemblies.

If you have two parts that can be assembled such that they are at 0, 15, 45, 90 degrees open, you set you standard assembly with one of these values. You then create several instances of that assembly the the angle dimension as the value in one of the columns of the family table. You could then use these instances in other assemblies that will show the parts in the various states of opened and closed.

Unless someone else know otherwise and can comment, the dimension needs to be controlled in the assembly in which it is made and not in higher assemblies.

Thanks, Dale

[wickmanscott]

Can't you do this with different states? You can save as many states as you wan't with different configurations and apply them individually to different views? You can use the 'Edit Position' button to rotate, or move the items you want. This has a downfall though as there will not be any constraints so it will be for graphical representation only?

[CamiloParraPala]

This is the best way to configurate assemblies http://learningexchange.ptc.com/tutorial/1480/creo-options-modeler-overview

[GregoryPERASSO]

Hello

Option Modeler (connected or not to Windchill Options & Variants management) is more designed for managing different Configurations of a product. (example Options for a Car), not to manage different "state" of the product

I'm not a ProE specialist, but if only have to manage angles, may be the "flexible" feature can be used to avoid creating Assemblies family tables.

You can also use Creo View Animation if you have licenses ... Not use it since newly released, but older Porduct View version works pretty well for this kind of need

regards

Gregory

[cgorni · Accepted solution]

To close this community thread on How to create multiple configurations (“states”) within an assembly?

• First note that Mechanism connections (or partially constraints components) could be used to:
  • Generate and display snapshots in drawings, as described in article CS30049
  • Connections can also be used to create animations

Summary of the exchanges and list of proposed alternate techniques (initial topic), also summarized in article CS136897

• Constraint sets with Family Table or Flexibility
  • Using constraint sets (defined when positioning the components), they may mimic the concept of configurations when associated to Family Table:
    • Create all variations of Constraint Sets in Component Placement for the parts you want to vary positions.
    • Add meaningful names to sets, like : Position_1 / Position_2 etc and enable only one
    • Create number of instances in assembly Family Table - as many as configurations that you need.
    • Add column items as Parameters > Look In: Component parameters, pick your component that have more than 1 Set and select PTC_CONSTRAINT_SET.
    • Add them per each component.
    • In the value for these parameters, put respective sets names in each cell.
    • Note: if you have nested structure (variations in different subassemblies) this will require creation of such family table at each level.
    • Bottleneck is that the instances will have different names than the generic when used in drawings or top assembly.
  • Flexibility could be used in association with constraint sets instead, as detailed in article CS46389
    • Flexibility can be defined in File > Prepare > Model Properties > change at Flexible row
    • PTC_CONSTRAINT_SET parameter of each varying component could be added
    • Or a global parameter could be created and used to control all them through relations
• Overloading the assembly to filter with Family Table, Simplified Representation or a Program
  • You could place the varying components multiple times at their different locations and enable/disable them using methods like Family Table, Simplified Representation or a Program
  • Family Table instances or Simplified representations offer the advantage to get parallel references to show in drawing views
• Placement Dimensions controlled by Relations, Program or Family Table
  • You can place your components with distances that represent dimensions that could be varied to achieve the wanted states, and even if they are set to be Flexible, see CS35523
  • However only one state at a time, in session, can be obtained this way. Therefore Family Table could used to create the different configurations

You can review the following threads too:

Assembly Configurations

Flexible Models vs. Part Simplified Representations vs. Family Tables vs. Constraint Sets

If you are more interested in configuring the Assembly structure (BOM variation) than the components position, you can review Creo Options Modeler capabilities and overview