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Transparent part option in drawing

Transparent part option in drawing

I'm working on an assembly that has some polycarbonate sheet as a cover. I'd like it if I could see what is behind the clear material in my drawing.

 

This is very different than wanting hidden lines - I do NOT want to see every hidden line of the parts behind the transparent material. I only want to see the next visible part, maybe as a lighter line, but only the visible edges.

 

It would be great if there was an option when you right click a part to set as transparent in the drawing - similar to toggling visibility or hidden lines.

 

transparenttransparent2.png

24 Comments
mrattray
Advisor

I think, in this case, you can accomplish what you need by turning of the visibility of your polycarbonate part.

Dan_Margulius
Advisor

Hi,

Until AD will think of this you can have a workaround.

Edit the view and pick "Shaded" style. you will have the same look as you have in the assembly .

Maybe you can do a new sheet and put on it Isometric view as Shaded. 

shaded.png

schnautza
Advocate
@mrattray - Turning the visibility off will make the edges of this part disappear. I still want to see the outline of it. @Dan.M - Our company plotter does not like the shaded views - everything is very dark with shading. I avoid shaded views when possible.
mrattray
Advisor

Another work around to consider may be changing your polycarbonate part's BOM structure to reference. In your view settings dialog there will be an option under model state for hidden line calculation. Set that to reference data separately and any parts under neath it will be shown. You can set line style to as parts in the same dialog to get rid of the reference lines. The "hidden" parts will show as visible lines. One problem with this is the polycarbonate parts wont show on your BOM when they're set to reference.

timdown73
Collaborator

Just a thought here...Shell the part (deselect the faces that you want to see through) by ohhh .001in.   That should be close enough to keep them from showing up as double lines on the drawing and still show in the BOM.  Density and volume will be incorrect though.

rjay75
Collaborator

This would be nice. One way I've simulated this is by creating a break out(s) using the profile of the transparent part in the view. I then set the break out to be from a point on the part and a depth of the thickness of the surface. Allows me to simulate transparency but keeps the parts in the BOM at the proper component types.

Scotty87
Contributor

This can be achieved using view representations and overlay views.

 

In the assembly, create a new view rep, turning off the visibility of the part to be transparent. Then in the drawing, place a base view of the assembly and select the new view rep as the view to be displayed. Click overlay view, select the base view, and then select the default view as the overlay. This will show the invisible/transparent part as dashed lines, and display everything otherwise obscured by it.

 

If you get a message about the lack of a positional rep, create a dummy positional rep in the assembly; this will allow you to continue creating the overlay.

 

Hope this helps.

dan_inv09
Advisor

I thought this was the place to ask for improvements, not get workarounds. (The shell thing and the breakout are probably the only ones that are close to being acceptable.)

 

We could also use something for expanded/perforated metal and similar things - but don't let that slow down work on transparency without shaded views. Thank you.

karthur1
Mentor

Totally agree with the idea.  There are workarounds to get you close, but they are just that.... workarounds.

 

 

dan_szymanski
Autodesk
Status changed to: Accepted

Accepted idea [US24903]. Thanks!

andrewdroth
Advisor

It would also be slick if apperances like grating and mesh displayed properly in IDWs.

timdown73
Collaborator

Grating and mesh would be good but I think it would need an option to simplify. If you had large areas of it, it could get messy.  I use symbols to show it now.

Capture.JPG

richard.koch
Contributor

At the end of my video i have a workaround for this...

 

thierry.osborne
Contributor

Hi there, I'm having the same problem, any new solutions (no workarounds please) to make the piece transparent AND stay in the BOM ? 

Quickcola
Enthusiast

I also wish I could make a part transparent in an assembly without affecting other assemblies.

Right now the part is transparent or not, regardless of it's use...

In solidworks, in an assembly, I can click a part and change its view mode for this assembly to transparent, without changing the material or view mode for the part anywhere else.

This permits me to see, work certain areas of assemblies, changing view modes for parts for current assembly, while not affecting the actual part or anywhere else it might be used.

mrhault
Explorer

I think my graphics card was failing, but it produced a cool result. I thought it was interesting enough to share.

Nice to have the ability to set specific parts to "clear", wireframe but no hidden edges.??

steve.west
Advocate

I get this occasionally, random part transparency. It comes and goes as you zoom in and out. Always assumed it was a software glitch.

steve.west
Advocate

I realise this is a bit of an ask, but a similar functionality would be useful where you have applied a mesh property yo the part from the material library. When drawing guards with mesh elements, I have to use a shaded view to show the mesh, or alternatively hide the part and sketch the mesh outline in along with a hatched 'patch' as I would in AutoCAD.

dan_szymanski
Autodesk
Status changed to: Gathering Support

Hello, this is a duplicate of the following Idea:

 

http://forums.autodesk.com/t5/inventor-ideastation/transparent-part-option-in-drawing/idi-p/3932644

 

Please cast your kudo to it as to not split the votes.  Thanks! -Dan

Som_Nohbdy
Community Visitor
Just one more workaround, my way to fix the BOM issues with a reference part: Have two .ipt files represent the transparent part. Use derived part to maintain a link for auto updating. Use both in the assembly (constrain their origin features to one another if you want to avoid constraint breaks when the part is modified). When you want the part transparent in the drawing, show the reference part & hide the non-reference, else hide reference and show the non-reference part. This preserves your overall BOM, weights, etc, but requires you to have an additional .ipt for when you want to show it as transparent.

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