Painting features in a single part file

[Superfly257]

Hello all,

Sorry to post what is probably an elementary question, I am new to Pro Engineer (I've only been using it for a little over a month now) and my problem is this:

I have a part file with multiple revolve features in it that are stacked on top of each other. So basically, if you imagine it similar to maybe a stack of washers... the top of the 2nd revolve is directly contacting the bottom of the 1st revolve, and the top of the 3rd revolve is directly contacting the bottom of the 2nd revolve, etc etc. I want to paint each individual revolve a different color so if you look at a cross section you clearly see the stack up (right now it just looks like a solid grey piece.) However, when I go to paint the surfaces, it acts as if all the different revolves stacked on top of each other are one solid piece and it paints one side of the entire stack up instead of just the one revolve I want. It doesn't seem to allow me to click the feature in the model tree in order to paint the whole feature at once, and if I change the selection method in the top right from "all" to "part" it again acts as if the whole thing is one part instead of many stacked features.
I also tried suppressing all the features but one in order to change the appearances one at a time, but when I paint the remaining feature and restore the suppressed features they are painted too.

This is driving me nuts!
I'm sure their must be a simple way to do this!

Thanks for your help!
Pete

 

[looslib]

If these are individual parts stacked up, model each one in a separate file and then build an assembly file of your stackup. You can then color each component of the assembly stackup.

Even if all of the components are the same, build one detail part file and stack them all in your asssembly file.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[Superfly257]

Thanks for the reply!

I guess I'll have to do it that way... is there really no way to do it in the part file though? If there is I would like to know how to do it both ways.

Thanks,
Pete

 

[jvian]

I believe you can do what you want at a part level using the split surface command and draw curves as break lines for the splits. This is similar to creating surface regions in Creo Simulate if you have ever used such. This feature does require an extension for use which I believe is the flexible modeling extension. Anyone correct me if I am wrong but I have done this in the past before the extension was required. I used it to break seeps which passed through a thin wall feature of a casting and needed access to the surfaces separately. I did lose that functionality (not sure when) but I know for sure it was gone when we moved to Creo 2.0 at which point it required the FMX. Without the extension you must use the assembly approach or use the assembly inheritance modeling which I think is unnecessarily complicated if all your after are colors.

Hope that helps,

- J -

 

[dgallup]

You can put a decal on the surface if all you want is a pretty picture. But Pro/E expects you to make your model the way you would physically make the part. It it is a stack of washers it should be an assembly.

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The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[mjcole]

Pete (Superfly257),

I think I know what you're getting at.
You've broken down a long shaft part into smaller sections so you don't have a single Monster Sized revolve feature. I've done so in the past and a few inside the box people couldn't fathom that choice. Obviously they never had to deal with laborious large sketches in ProE.

Well getting to the method you can use to achieve what you are looking to do.
while in the Part Color tool - select the flyout to apply color and when promted to select something to color hit ^F or CTRL+F and you will get the search tool Finder the Binocular looking icon linked below because Google Photos images decided to no longer show or use extensions for images and the photolink fails.
[url=https://plus.google.com/u/0/photos/101396575104457719372/albums/5109325364883017297/5855020740114783490Search Filter - AKA Finder Tool[/url]

Once you get the finder open make sure the [Options] Button has "Build Query" checked on
Doing so will give you 5 buttons to [Add New] [Remove] [Update] [Move Up] [Move Down] list

The finder tool allows you to paint the surfaces involved in each of your surfaces a different color. In Proe Creo PTCsNextCADdesignation. Color can be applied to the entire solid model [Part] color is the first thing set and all features will be painted that color when made. After that in the higherarchy comes Feature color which can be applied by coloring all the Faces of your feature.
For Second criteria use Feanture by Type and select revolution or just Feat.ID or Number
to make your life easier you can display Feat # and ID in your Model Tree to help out.

You can use a variety of search criteria or just one.
If you want a base color you can search for Solid Geometry using the All (radio-button)found on the history tab [History] tab or Right Click with Geometry in selection filter and select All Solid Surfaces.
Surfaces: can be classified as individual faces on a solid or one of the patches on a
Quilt(continuous surface body connected surface)
Filter Rule Summary

Then to color your features use. -See Image linked above
Look for: Surface
Look by: Feature
[Attributes]
Rule: Type
1 Comparison: is equal to
2 Category: Creation Method
3 Value: Revolved
or you can use the following to include extrudes and other sketch based features.
2 Category: All
3 Value: Protrusion

Give a look at the possible search by optihns to learn more I hope this will make your task easier to accomplish.
Search By
[Attributes]:
[History]:
[Status]:
[Geometry]:
If you'd like me to make a FAQ about this on the site let me know in response to this post.
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