Part color is not updated in the assembly

[Anonymous]

When I create an assembly file, I added the part files I want and they all looked normal. But after that, whenever I create a new solid in my part file and change the material/ color, the material/ color changes won't appear in the assembly file. The new solid will appear in the assembly file but the material will just be the default setting even when I have already changed the material in the part file. I'm using Inventor 2019. How do I fix this?

Thanks

[SBix26]

A part file (.ipt) has only one material, shared by all solid bodies.  You must be changing the appearance of individual bodies.  Is it possible that you have more than one Design View Representation in the part file, and that you're changing the appearance in a Design View that is not the one in use in the assembly?

If you can zip together and post the assembly and components, maybe someone here can figure out what's going on.

---

Sam B
Inventor Pro 2021.0.1 | Windows 10 Home 1903
LinkedIn

[Anonymous]

@SBix26 Thanks for you reply! I'm not sure whether I have the same design view for both files. I posted my assembly and part files in the attachment. The part file I mentioned was named "Cavity". The default material there was cooper.

[Anonymous]

If you clear the assembly colour overrides, the part colours should show.

To do this, select all of the occurrences in your assembly file, then choose "Clear Override" from the override browser, as shown below

[SBix26 · Accepted solution]

As I suggested, the problem is with different design views.  In Cavity.ipt, there are seven different View Representations, and the active one in that file is called HolesSection.  However, in the assembly, the selected View Representation for Cavity.ipt is Master.

If you open Cavity.ipt and switch VR to Master, you will see it just as it is in the assembly.  Or, if you right click on Cavity.ipt in the assembly and select Representation...  and then select HolesSection, you will see it as it is shown in the part file.

One other thing: the part file will not look exactly like the assembly file, because they are using different lighting styles.  The assembly uses Two Lights and the part file uses Grey Room, which give quite different results for the same appearance.

In the end, it seems that appearances were assigned to the new solids in Cavity.ipt while HolesSection was active, so they are unique to that View Representation, and not to others.  If appearances are assigned in the Master view rep, they will carry over to others as well.

---

Sam B
Inventor Pro 2021.0.1 | Windows 10 Home 1903
LinkedIn

[johnsonshiue · Accepted solution]

Hi Michelle,

This can be done fairly easily. Simply open the assembly and select the part -> right-click -> Representation -> pick a desirable Design View Rep in the part -> check the associative box. From now on, any change to that particular DVR in the part will be shown in the assembly.

Many thanks!