IDW drawing with frame as hidden line and decals on frame as color shaded

[Anonymous]

Hello all, I may sound stupid but I want to ask you question.

I have a frame with decals on it. someone before me did the drawings and somehow he manage to make frame as hidden line styles but the decals are as it in model file, colored shaded.

I have attached the screenshot for better understanding of my question.

I check the model file, frame in model file has appearance as "CLEAR". that's it, all other options are normal as default.

 Thank you.

[mcgyvr]

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@Anonymous wrote:

I check the model file, frame in model file has appearance as "CLEAR". that's it, all other options are normal as default.

 Thank you.

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Ok and did you try assigning that "CLEAR" appearance to your frame then creating a drawing?

Can you post the drawing file?

And please go ahead and give "kudos" to this idea for a future improvement to Inventor to make it easy to accomplish this in the future..

https://forums.autodesk.com/t5/inventor-ideas/show-decals-in-all-drawing-view-styles-not-just-shaded...

[Anonymous]

Yes, I did try that clear for frame but even in drawing, it still comes and show clear effect, its not as it in that hidden style.

I want to upload but its my company's property and don't want to mess by uploading confidential file.

[Curtis_Waguespack]

Hi paf_redstars,

Can you provide screen shots of the browser, specifically of the view in question.

My guess would be that:

A) there is a sketch on the view, that contains the decals

B) there is an overlay view using a combination of View Representation and Positional Representation containing the decals (this would be less likely).

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

[bshbsh]

Possibly the frame is set to reference or phantom in the assembly BOM.

[Anonymous]

THE BROWSER SCREENSHOT OF THAT VIEW

[mcgyvr]

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@Anonymous wrote:

Yes, I did try that clear for frame but even in drawing, it still comes and show clear effect, its not as it in that hidden style.

I want to upload but its my company's property and don't want to mess by uploading confidential file.

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You need to select "Hidden Line Removed" from the style section of the base view dialog box..

I assume this is your first Inventor drawing? 

If not please do the following..

#1-Set your frame to that same clear style

#2-Place a base view with "Hidden Line Removed" style option checked..

#3-Take screenshot of that drawing view and post here..

[Anonymous]

Screenshot of hidden line remove style and what person before me did. Clear can see that reflective warning decals are colored in his way and not colored in what you ask me to do.

[bshbsh · Accepted solution]

This is how I do it:

(note: I just threw in two random parts/assys, I don't have any actual decal, but it should work the same way)

In the assy, set your Frame to BOM Structure: Reference, decal as normal.

On the drawing, set your View to shaded, hidden line removed. On the Model State tab, set Hidden Line Calculation to All Bodies, Line Style as normal, Margin to something big so it doesn't clip away the ref. parts lines.

Finally, on the drawing, find the view in the tree browser, expand the assembly, right click on your Frame and you can select a custom line style, eg. thin lines.

[Anonymous]

Thank you so much. you are a life saver.

That's my first time here, asking question, and got solution within 2 days, really love this community.

I have marked it as solution and also give it a KUDOS 🙂

Thank you again.

[mcgyvr]

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@Anonymous wrote:

Thank you so much. you are a life saver.

That's my first time here, asking question, and got solution within 2 days, really love this community.

I have marked it as solution and also give it a KUDOS 🙂

Thank you again.

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If that works for you then fine..

Its not a good workflow though IMO..

Now your BOM/Parts list is incorrect as your frame is marked as reference..

If its really reference then fine.. But I doubt it is.. 

And normally we do much better than 2 days... But this is just something Inventor really doesn't do out of the box.. Hence my "ideastation" request to add the needed functionality.. 

[bshbsh]

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mcgyvr wrote:

If that works for you then fine..

Its not a good workflow though IMO..

Now your BOM/Parts list is incorrect as your frame is marked as reference..

If its really reference then fine.. But I doubt it is.. 

And normally we do much better than 2 days... But this is just something Inventor really doesn't do out of the box.. Hence my "ideastation" request to add the needed functionality.. 

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yes, that's a drawback indeed, but in his screenshot he was using a shrinkwrap so i assumed it's kinda like a separate drawing for illustration purposes only. and because of how that shrinkwarp is represented on his drawing, and also not having a item number balloon, I'm almost certain it's set to reference bom too, I can't think of an other way to achieve this. (but let me know if there's one)

and as a workaround you can insert the "reference" part twice into the assembly (on top of each other), one is set to reference BOM, the other to normal, and use two design views for the "normal" view (with the reference part hidden) and the "lines-only" view (with the normal part hidden). that way one could have this kind of a representation on the proper drawing with proper BOM. it's kinda fussy but at least doable.

in cases where I had to do this kind of a representation, it was actually a requirement that the parts list only show the "shaded" parts (and no manual overrides or hidden parts in the parts list), so setting the others to reference was a proper solution.

but yes, inventor lacks many features indeed.