Family Table Color

[wfalco]

All,

Up to Creo 3.0 - whats the latest and greatest solution for having instances being differing colors?

I recall seeing something in the past that may have involved adding surfaces?

But I just bet it's easy in 3.0.........................NOT! LOL.

WayneF

[AmitDeshpande · Accepted solution]

Hi Wayne,

I found an article that may address the issue.  Please take a look at the following:

CS33983 - Is it possible to assign a different color for each family table instance using Material Appearance in Creo Parametric?

If you are unable to access the information, the resolution listed is as follows:

• Intended workflow
  • Assign material to a part (material contains an appearance)
  • Multiple materials can be added to a model, but only one is active at a time
  • PTC_MATERIAL_NAME parameter can be used to switch between these materials and the color will update accordingly
• The problem occurs when this parameter is used in family tables and multiple instances are in session
  • Reported to R&D as SPR 2067440
  • There are plans to implement this in a future release of Creo Parametric (a specific release has not been confirmed)
  • You can vote for Product Idea 5073
• Workarounds exist but are not guaranteed to work so avoid using them if possible and test with non-production models before using either one
  • Workaround #1: create surfaces and assign appearances to them
    1. Copy and paste all external surfaces as one feature in the generic model and assign an appearance to it
       1. Selecting one surface in the model
       2. Right click and select Solid Surfaces
       3. Click Ctrl+C then Ctrl+V
       4. Click the green check mark from the dashboard
    2. Repeat step 1 for each color needed in the family table
    3. Add the surface features to the family table and set each feature to Y or N to get the desired color for each instance
    • This takes some manual effort but will be more stable is the model design is finalized
    • If features are added to the model, the appearance assignment may need to be repeated
  • Workaround #2 (use the intended functionality but don't have two instances in session)
    • Assign appearances to materials in the material library and use PRO_MATERIAL_NAME parameter in the family table
      • See article CS31202 "How to control the color and appearance of a part automatically based on the material assigned"
    • This method has proven to be unstable
    • Best results have been achieved when
      • The generic model does not have an appearance assigned to it
      • The instances are not in session when the family table is being configured
      • Only one model is in session at a time
        • After configuring the family table close all models and erase session memory
        • Open an instance to check its appearance
        • Close and erase session memory before checking another instance
• Note: The workarounds are not supported by Creo View and so the defined colors will not displayed correctly if published or viewed in Creo View

Thanks,

Amit

[wfalco]

Thanks Amit! I copied surfaces and tabled the surfaces.

[ptc-5132323]

There is another Workaround #3:

- Add a extrusion that removes the existing solid

- Add features that copy the original solids

- Paint the new features in the desired color

- Modify the table to suppres these features

Comment 1:

Make use of a component interface on features who are never suppressed to avoid problems when replacing parts.

Comment 2:

You can modify the program of the part to avoid a lot of collumns in the family table. This way less errors can be made when adding a extra component. For example, if "BLACK" is in the Parameter "TITLE", unsuppres the following features.