How to control the model color for family instances

I would not use a family table for this.

If you need the same part geometry that is a different color in Creo then use the part design model and merge the geometry into a derivative part for each color. For each derivative color assign the color to the part model and save it. All colors will have geometry driven by the master and will present the color assigned in Creo assemblies.

Is it required that you have Creo models of the same geometry that are different colors? If not then you can deal with this by tabulating the drawing by using suffix on a common part number. For example C123456 is the p/n and suffix -01 is white so C123456-01 represents a white part. You can use a table on the drawing to add any new colors as required in the future.

You can assign a different color to every material in Creo.  You SHOULD be able to copy, say, aluminum 6061-T6 as 6061-T6_RED, change the color to red and then assign that as a material ("PTC_MASTER_MATERIAL" parameter column in the family table) to the instance....BUT, PTC STILL hasn't fixed that glitch.  It's SUPPOSED to work that way, and actually DID once back in the early Wildfire days, but after that and even now (and I just tested it), it doesn't work.  If you make the generic aluminum with it's stock silver color, if I make an instance that's brass (you have to open the instance to assign the material, it's difficult to do it in the table), then it changes the instance to that material and color, but when you go back to the generic it's the proper aluminum material but takes on the brass color!  I know of no fix.  You MIGHT be able to do it by creating a multibody part and make a copy of the body and assigning that body the color, but I'm not sure how that would work out.  I guess you could make a surface copy of the original part, then do a solidify cut to remove the original body so that only your new body with it's desired color is there.  Suppress the solidify cut as needed.  Rinse and repeat.

The material swap would be the PERFECT and easy way to do this, but, as I mentioned, it's been broken for, geez, 15 years now, like not being able to see cosmetic threads in the model unless you switch to wirefram...aaaannnd they're in no hurry to actually fix it.  But hey, we get a new and ever MORE confusing ribbon every year, RIIiiigght?

Best of luck...

There's an ugly workaround by using quilts or a zero value offset feature. See this thread:

https://community.ptc.com/t5/3D-Part-Assembly-Design/how-to-change-color-of-a-part-using-relation/td-p/291474

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@MB_10357724 wrote:

I want to assign different color for each family table instance. is there a way to do this? pls suggest.

 

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Hi,

I am not 100% sure but it seems to me that in the past I was able:

• assign 2 different colors to 2 different materials
• assign above mentioned materials to 2 different family table instances
• start Creo and open instance no.1 showing color1 ... then closing Creo
• start Creo and open instance no.2 showing color2 ... then closing Creo

Unfortunatelly you cannot assemble 2 above mentioned instances into the same assembly !!!