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anagnost1-Visitor
1-Visitor
November 25, 2011
Question

Model color schemes

  • November 25, 2011
  • 15 replies
  • 20446 views

Hello all,

is there any way (or workaround) to define various color schemes for a part or assembly model?

For example, when we are working on an assembly, we use different colors to distinguish the different components. Also, at the same time and when we have to make some rendered representations, we have to define some other colors in order to simulate reality as close as possible.

Any ideas? How can someone switch from one color scheme to the other?

Thanks in advance.

Vassilis Anagnostopoulos




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15 replies

BrianMartin13-Aquamarine
13-Aquamarine
December 13, 2011

Hi Vassillis...

Hmm... I've seen model colors change before when a different color map file was loaded (back at Wildfire 2 and 3). I forcibly TRIED to make that happen just now in Creo Elements Pro (Wildfire 5) using two different appearance files and couldn't make it happen.

It's supposed to be that colors are saved with the model. But in the past it was possible to name your colors, load a new appearance file, and then OVERWRITE those named colors with new ones. I've seen this change the model colors on the screen before in WF3... but I can't make it happen now. This makes me wonder if the instances I witnessed in the past were bugs... or if I am mistaken that it was ever possible in the first place.

I'll keep digging... stay tuned.

thanks!

-Brian

BrianMartin13-Aquamarine
13-Aquamarine
December 13, 2011

Hi again...

Yuck. Here's what I found:

I was able to swap colors on models by applying colors to my materials and setting the config.pro option mat_assign_appearance to yes. Using a simple dummy material, I assigned a color of blue giving it a name "material_color". I saved this color from the MATERIAL input window as global_blue.dmt. The global appearance file supercedes the normal model appearance file... so I used this to help achieve the color swapping effect.

I went back to the same material, changed the color to green but kept the name of the color set to "material_color". From the MATERIAL input window, I saved this appearance file as global_green.dmt. Now I have two color files assigned to the same color name.

When global_green.dmt is active, the color called "material_color" is green. When I load global_blue.dmt, the color called "material_color" is blue. I can swap between the two color files and my model changes color (not quite automatically but close enough). In practice, this would be awfully tough to achieve.

I tried a variety of other ideas. I tried UNASSIGNING all materials hoping the model would revert back to it's original color. It did not. I tried saving two appearance files with different color palettes and loading them over top of each other (in an attempt to overwrite the colors). This failed.

In fact, loading the same named color over itself caused Pro/E to throw out a message warning me I was changing my color palette. I accepted this and told the system to overwrite the old palette with the new one. Yet the OLD palette stayed active until I physically clicked on each color from the palette. Once I clicked on the old colors, they disappeared and the NEW colors popped up. Weird. Definitely buggy... very buggy.

I hate to leave people with a NON answer and no possible solution... so I have to give you something. In a pinch, try these:

- Create a new assembly ONE LEVEL HIGHER than your current top level assembly. Add your top assembly as the only component. Color your assembly there for final rendering. This allows you to leave the colors alone in your current top assembly and create a different look to your part for rendering.

- Assign a string variable called "render_color" to each part in your assembly. Use that parameter as a selection device using the FIND tool. You could select all objects with the "render_color" set to "blue" easily using the find tool. Apply your rendering colors this way to save time. You might even be able to use a mapkey to speed this up.

- Play around with the material appearance assignments. they aren't great but they do offer some hope of toggling colors at the part mode quickly (when they're working properly... I had a few issues with having to re-issue the commands several times before the system responded).

Sorry I don't have better advice... anyone else got anything?

Thanks!

-Brian


DalbeerSinghSoh1-Visitor
1-Visitor
December 14, 2011

there is a way to do it which i often use, make seprate part/assembly for rendring. all u have to do is to copy all surface and publish thoes sufaces and call publish geometry in new part by copy geometry. This way u can keep both color schemes... and dont worry about changes that u will made in part or assemble it will automaticaly update.. try it and let me now

one.jpg

Thanks

- Dalbeer

Message was edited by: DalbeerSinghSohal

    BrianMartin13-Aquamarine
    13-Aquamarine
    December 14, 2011

    There are some shortcuts to using this technique Dalbeer is suggesting.

    You can create a Shrinkwrap which will automatically gather all solid surfaces of your assembly and all sub-levels (or selected sub-levels) into one object. If you create an External Shrinkwrap, you can keep the new model separate from the existing assembly while preserving associativity.

    To do this, you have to create your shrinkwrap from the Insert>Shared Geometry>Shrinkwrap menu. You can't do it properly using the File>Save a Copy menu to save your shrinkwrap.

    There are problems with this technique, though. In Dalbeer's method, you create MULTIPLE copied surfaces. Each one represents one part from your assembly. In my method, you avoid having to copy surfaces manually, create publish geometry, and then create external copies. However, the downside is that my technique creates ONE copied surface with sub-features representing each part in the assembly.

    Both techniques appear to give the same result. Mine is faster and more automatic but with Creo Elements Pro (Wildfire 5), it's harder to assign colors to my copied model. Dalbeer's is easier to color because he has individual features. Mine are all lumped under one feature which still should be easy to color but the software really fights you when trying to select surfaces.

    Ideally, you'd combine the two methods. If you make one separate copy/shrinkwrap feature for each component in your assembly, you'll avoid the selection problems my method has. If you use External Shrinkwraps or External Copy Geometry, you'll avoid carrying copied surfaces and publish geometry in your top assembly.

    None of these suggestions gives us what we really need... "Appearance States". We need the ability to keep multiple appearance settings in the same model and toggle between them. We have Layer States, Simp Reps, Style States, and a ton of related features but we don't have Appearance States yet and that would be the best solution to your problem.

    Thanks!

    -Brian

      anagnost1-VisitorAuthor
      1-Visitor
      December 21, 2011

      Dear Brian and Dalbeer,

      thank very much you for your time and effort.

      Yes, both of your techniques can give some results but unfortunatelly they are not so easy to use. Imagine how much time you need on an assembly with some hundreds of components...

      On the other hand, I believe that it's not a bad idea to have the ability, to define various "Appearance States" for a model.

      thanks anyway.

      Vassilis

      PS. What do you think about a poll questioning about the necessity of this functionality?

      JavierGarcia10-Marble
      10-Marble
      December 16, 2011

      Hi, i suppose you have already tried this technique:

      http://www.imakenews.com/ptcexpress/e_article000650263.cfm?x=b11,0,w

      I have used it sometimes but would like Pro/Engineer to offer a feature to handle this.

      BrianMartin13-Aquamarine
      13-Aquamarine
      December 22, 2011

      Hi Javier...

      Thank you for the link to that article. This technique is similar to the one I suggested using the material color options to create different appearances based on material type.

      Best regards,

      -Brian

      Patriot_1776
      Patriot_177622-Sapphire II
      22-Sapphire II
      December 23, 2011

      Probably the best and simplest way to do this without having to create shrinkwraps and all this external references is to make family table parts of all the parts and assemblies that will change, create different materials with different appearances, and swap them out as needed. The parameter: "PTC_MATERIAL_NAME" (if I remember correctly) is a parameter column where each cell value can be swapped out in each instance in a family table, and then just swap out the part at the assembly family table level.

      Depending on version, there's a glitch in the software where it doesn't work (WF3) or requires 2 regens (WF4) to work.

      BrianMartin13-Aquamarine
      13-Aquamarine
      December 23, 2011

      Hi Frank...

      There's actually a glitch in Creo Elements Pro (Wildfire 5) where this ALSO isn't working right. The material appearance thing is really buggy (at least in M090 of Creo Elements Pro).

      The other problem with using a family table is model size. If this is a small-ish assembly, tabulating each part and sub-assembly might make sense. But if Vassillis has hundreds of parts, he's going to have to create a real rat's nest of tables and instances to make this work.

      There should be something easier... but unless we have a Pro/TOOLKIT guru out there somewhere, I'm not sure of a better way. 😕

      Thanks...

      -Brian

      Patriot_1776
      Patriot_177622-Sapphire II
      22-Sapphire II
      December 23, 2011

      Imagine that, a glitch......

      I think in that case, the entire sub-assembly of 100 parts could have a material assigned to the assembly, that each individual part wouldn't have to swap. The model size isn't as big an issue as you'd think, it's actually just a text file within the generic.

      I wish they WOULD fix the appearance of the materials, I was trying to make a big family table of fasteners and wanted to show versions of sizes in stainless, brass, black oxide, etc. In WF4 I SORT of got it to work, but had to regen twice, and it was still wanting to change the instances to whatever the generic looked like.

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