Assign different color to a family table component

This has been covered. You can create different materials with different appearance (but same mechanical properties), and then assign different materials to different instances. You must load all the different materials first in the generic, and then add the parameter "PTC_MATERIAL_NAME" as a column and swap out the different materials for the different instances.

Bill,

today I read the following information:

1. Select the required colors for the respective material by using menu selection

File > Properties > Change Material > Double click on the required material >

Appearances Tab > Chooser > Select the required Color > OK >#OK.

2. Note that no color is assigned to the generic part the PTC_MATERIAL_NAME

for generic should be UNASSIGNED.

3. Select the parameter PTC_MATERIAL_NAME as the variant for the family table

and then select the required material for each of the instances.

Martin Hanak

Hi folks,

If you need to add diferent color for your components and do you want to use Family Table, you can create on your Generic model Surfaces Copy feature (as Solid Surface copy = select surface>RMB>Solid Surfaces >> CTRL+C >> CTRL+V -> enter)

Change name in model tree (you can set same name for copy feature as your color).

You can create many of copy geometry features and then set diferent colors for Quilts (created surfaces).

In Family table you can select features (Copy geometry) and set "visibility" for your instance models.

Regards,

Vladimir

Hello, a few years late to this thread but maybe someone still faces the same problem. We have Creo 12.4. and I managed to assign different colours to instances of family table.

What you need to do first is that you assign a colour to the every material you’re planning to use. Once you got this covered, you go to the generic part and you add all those materials to the model. You should not set some material to master, leave it as it is.

In model tree under the Design Items expand Bodies and here you have to assign a material to body, not to the model itself. (see screenshot below)
 

After that, you can create a family table. Add columns → choose parameter → and here in the Look In tab you have to select Body (see screenshot below)

Once you select look in to body, you have to click on your body in model tree for a parameter to appear in selection box.

You confirm selection with Insert Selected and then you just add instances to the family table and from the drop down menu select the material you need.

To my knowledge this is the only way to display different colours in instances without a bug.

Hope this helps :)

You USED to be able to assign different materials (with their different colors) to different instances, in early Wildfire I think it was, then in later versions of Wildfire it stopped working and hasn’t worked since.  I’d given up on PTC actually fixing this and don’t play with bodies too much.  I’ll have to try this and see if it works, thanks for the Pro/WORKAROUND (Old insider joke).

Hi

I am on Creo 10.0.9.0.

I tried the method used by Vladimir and it works perfectly. There is no need to assign different material.

I added a “Restricted” parameter “Colour” and assigned different colours to it. Added the Parameter to the family table for Leader Notes indicating colour. The following picture should explain the process.

The material is as defined in the generic part.