Component Display in Drawing not working.

[MikeMarcoux]

In Creo 2 Parametric, I'm having an odd issue. I've done this a thousand times in the past without issue, but for some reason, it is no longer working.

In an assembly drawing, I'm attempting to use component display to blank and change some components to phantom transparent, but after I select the components and style, nothing happens. The assembly remains unchanged.

Is there a new config setting I'm missing in Creo 2?

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[TomD.inPDX]

I have had to regen and even re-open the drawing in some versions for the entire change to take place.

[MikeMarcoux]

I thought the same thing, but it still remains unchanged.

[SYNDAKIT]

AFTER SELECTING THE OBJECTS I ALWAYS HAVE TO CLICK "DONE" FOR THAT STYLE TO APPLY. IF I JUST CENTER CLICK OUT OF IT, IT WONT APPLY THE SETTINGS.

[MikeMarcoux]

That's the way i've been doing it Joe. It's really odd. I've even tried it across multiple assembly drawings. No dice.

[TomD.inPDX]

Is there something special done to this component such as assembly cuts or whatever? You could try to add the part to a test assembly and open it in a drawing to see if it functions correctly.

I have not run into limitation as yet with this function, but you may have found one.

Feel free to post the components; let us know the version it came from; and to know if it is from the full or academic version.

If you have maintenance, of course, open a support case and have PTC look at it too.

[MikeMarcoux]

Will do.

I'm running Creo 2.0 Parametric, M070, full version.

I've actually tested this on several different assemblies, and it doesn't work on any of them. That is why I was wondering if I missed a config setting. There are no assembly cuts in any of the models. I've used this feature so many times in the past without issue. I'm wondering if there is a new config setting, but I've searched and have no found anything pertaining for item display in assembly drawings.

[TomD.inPDX]

This is the case will all the components or just a particular one?

I just open an old assembly in a new drawing in Creo 2.0 M040 and it is working as expected. I can blank things and change their style without issue.

I am also going to assume you are not using combined states settings when defining your views. Not that I know if this is a limitation.

[MikeMarcoux]

All components. No combined states. I'm really at a loss on this one.

[TomD.inPDX]

Can you submit this as a support case? PTC may already have an answer to this.

[MikeMarcoux]

I think it's the only thing I can do at this point.

[MikeMarcoux]

Things just got really interesting. Blanking and unblanking components works on one view, but changine style to phantom transparent or opaque does not. And? It only works in one or two views, not any other view.

[TomD.inPDX]

This is where IT comes in and asks if you reformatted your drive yet

If you want me to have a look at your files, I would be happy to. It could always be that your Creo installation is corrupted somehow. Support can link to your computer and help trouble shoot this, but I suspect they will need to duplicate it on another machine to get it to R&D. If this is your machine only, be prepared to re-install or repair your Creo installation. You can have support on the line while this is being done. They may also try cleaning out some cache folders.

Do you still have the virgin boot option (default install shortcut) available so no custom configs show up? It is worth a try to see if it is something in config.pro or alike.

[MikeMarcoux · Accepted solution]

What's odd, is that I just went through support recently for a separate issue with Solidworks and Windchill. (we run both Creo and SW here). They found the problem and fixed it, so hopefully the can pull this one out as well.

We do have a custom config, and a startup script that pulls the same company standard config for everyone, but it's the same config we've used forever. I have no problem dumping a cache or even blowing it away, but the odd intermittent nature of this one makes me thing it's something else.

Thanks for all of your help. When I get a solution, I'll be sure to post it up.

[TomD.inPDX]

Thanks Mike. Good luck!

[MikeMarcoux]

I've figured out the source of the error. As it turns out, component display does not work for drawing views that are shaded or shaded with edges. The view must be no hidden, hidden, or wireframe. I feel like I should've known this, or maybe did know this and had just forgotten about it.

[TomD.inPDX]

Well, that was a given from the start

Shaded was a late addition and you cannot shade a section either.

Since shading is a huge requirement in my work, I use assembly cuts for a lot of my drawing views.

Since you are also using shaded views... here is a tip: Place a shaded view (no edges) and lay a hidden (wireframe) view on top of this. This way you have control over those "edges". By default, it is only slightly different, but different none the less.