1 part, 2 color options

[ToddPig]

I would like to add a view of my part to my drawing that shows the textured surfaces.  In Solidworks, I would create a configuration (named "texture" for example), then I would highlight (or change the color) of all the surfaces that require a certain texture.  I would like to do this or somethign similar in Inventor.  Is the only option to use iParts?

Thanks,

Todd

[mdavis22569]

Like this ?

[ToddPig]

Mike,

No. Let me give more details. I have a clear plastic injection molded part that I would like to show the textured surfaces. I would like it to be clear for the first 2 sheets of the drawing, and in it's assemblies, but would like the option to turn on or off the colored surfaces.

[mdavis22569]

yeah I'm going to step back on this one ... this would probably be something JDMathers could answer. I haven't been on Solidworks since 2009

[Curtis_Waguespack]

Hi ToddPig,

If you're wanting the entire part to be one color and then the entire part to be another color you can do this by creating View Representations in the part file and use those to hold the color changes. Then you when you place the part into an assembly you just need to specify which View Representation to use. And/or when you place views on your drawing sheets you specify which View Representation to use:

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014...

However, if you want to have your part with the front face red in one View Representation, but have only that same face blue in another View Representation, I don't think that can be done in a single file, as the color overrides applied to individual faces push through to all View Representations (unless I'm remembering incorrectly).

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[ToddPig]

Curtis, thanks for the reply. I was looking for what you described in your second paragraph.

I think I'm going to have to have 2 parts (maybe even a derived part) to accomplish this. Kind of frustrating to keep being reminded how much Inventor is lacking when compared to Solidworks.

[Anonymous]

View Representation in Inventor are the Same as Configurations in SolidWorks.

[ToddPig]

Nope!

In SW I can do exactly what I am trying to do (this is a standard process for many of my customers), in Inventor I can not do this (thus why I asked the Forum for help and ideas).

[Anonymous]

Have you even tried? You can have multi view Reps in your part and each view rep can have a different color or texture.

Don't tell me I wrong I have been using Inventor for many years.

[Curtis_Waguespack]

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@Anonymous wrote:

Don't tell me I wrong I have been using Inventor for many years.

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Hi Doug_DuPont,

You're not wrong. But I think the original question wasn't clear, here's is my understanding of the request:

Let's say we have a gray cube and we want to show this cube on sheet 1 of the drawing in several views detailing it out, but in every view we want all of the sides to show as a gray cube.

Then on sheet 2, we want to detail out the cube, but we want to color code / highlight the top face as red, all other faces to be gray still, and have the top face be red in only the views on sheet 2.

Then on sheet 3, we want to detail out the cube, but we want to color code / highlight the front face as blue, all other faces to be gray still, and have the top face be blue in only the views on sheet 3.

Can we do this? I might have overlooked it, but I was not able to use part view representations to control individual faces, without the color changes pushing through to all view representations in the part, and therefore pushing through to all of the views in all of the sheets in the drawing.

We would also want to show only the red face in one assembly, and only the blue face in another assembly (or another view representation of the same assembly).

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[swalton]

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@Anonymous wrote:

Have you even tried? You can have multi view Reps in your part and each view rep can have a different color or texture.

Don't tell me I wrong I have been using Inventor for many years.

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As I understand @ToddPig's issue, he wants to change the color of some, but not all, of the faces of the part and that the color and faces need to change with each View Rep.  My experience is that View Reps don't work like that in Inventor 2014.  

As discussed in @Curtis_Waguespack's 2nd paragraph, above:

View Reps behave differently if you override the color of a set of part faces, rather than if you change the Appearance for the entire part.

My quick testing showed that View Reps will honor the assigned colors for each body of a multi-solid part.  Try using the Split command to create separate solids for each required color change.  RMB on each body in the graphics window or in the Solid Bodies folder in the browser and select Properties.  Use the drop-down in the Body Property window to override the Body Appearance as required for each View Rep.

[Frank-Oosterwaal]

Hi.

I don't know how complex the surfaces are that need the color change but you could use offset surface with "0".

Then change the color of the surfaces and make different view reps with the surfaces on or off.

This seems to work:

[ToddPig]

Curtis, this is exactly what I am trying to do. I was able to accomplish this using a derived part, but it seems like more work than necessary.

[ToddPig]

This is exactly how I used to do this in SW roughly 7 years ago, then I was able to handle the issue with configurations, and it was much easier.

[Frank-Oosterwaal]

Yeah, It's only a workaround.

I don't think there is another way in Inventor for now...

[Curtis_Waguespack]

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@Frank-Oosterwaal wrote:

Hi.

I don't know how complex the surfaces are that need the color change but you could use offset surface with "0".

Then change the color of the surfaces and make different view reps with the surfaces on or off.

This seems to work:

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@ToddPig wrote:

This is exactly how I used to do this in SW roughly 7 years ago, then I was able to handle the issue with configurations, and it was much easier.

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Hi ToddPig,

If that's how you did it in Solidworks, then I can confirm that you can do it with Inventor, using the offset surfaces and controlling them with part View Representations. It's not as tidy of a workflow as I'd like to see , but it looks like it can work.

Keep in mind that you will want to the surfaces not to be Translucent (right click on them). Also, I have better luck with surfaces displaying properly when I offset at something like 0.001 rather than zero.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com