I have an assembly with 5 different components and I'm planning to create 7 different instances. 4 of the 5 components will always be painted the same color, but the 5th component needs to be a different color (color-coded for each of the 7 instances). When I assign that component a color in the generic assembly, the same color propogates to each of the 7 assembly instances.
Anybody know how to overcome this problem?
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.
Frank.....I really wish it was that easy. I've tried your suggestion many times before but there always seems to be a regeneration problem (with appearances). One of three things ALWAYS occurs:
Yup, you too found a bug in the core functionality they haven't fixed for years. Too busy making ribbons I guess......
Yeah, it's frustrating. Usually a second regen does the trick. In WF3 it didn't work at all, in WF4 is worked as you see it now. Are you in creo> I haven't tried it there yet....
OK, glad to hear I'm not the only one who has experienced this.
We're using WF5 actually, but yes, I had the same issue in WF4. The Appearances functionality has always been (in my opinion) one of their worst features.
Yep. I had this really neat family table of fasteners in various materials (stainless, black oxide carbon steel, zinc-plated carbon steel, all color-coded materials, and it never worked the way I wanted it. I thought that would be a great visual to the Engineer or Designer to see if they had the right fastener for the environmental conditions. I even did o-rings like that, but it never worked the way it SHOULD have if it wasn't buggy.
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.
This is precisely how I set up my family table, but it does not work. When I open a part (whether it's the generic or an instance), it always adopts the most recent color in memory (PTC_MATERIAL_NAME).
Once in a while a regeneration might work, but it's only temporary.
I have also tried creating different material and assing them to different instances of family table. When more than one components of family tables are assembled in same assembly, it shows only most recent color.
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.
just one note ...
It seems to me that in the past, ProE mixed the color of solid face with color of quilt surface, when user used this trick. Stripes of both colors were displayed instead of quilt color.
Hi Martin, it is working correctly - I have tried it with ProE Wildfire 2.0 too