IDW-Is there a way to display a single part as hidden lines like reference parts

[rcolon9E4ZX]

Hello all,

I am making a drawing of an assembly. I have multiple views of this assembly. In one view only, I am looking to display a part as hidden lines, much like what setting the part as reference does. This part is behind other parts. I would simply assign the part as reference, but I do not wish to see the part as hidden lines in all the other views, and this removes the shading of these parts in these views.

Setting the part that is blocking the part in question to transparent reveals too many lines and makes the view confusing. Is there a way that I can select a part and change a property to make it visible on top of all other parts, with the ability to set the line type as dashed?

Many thanks in advance.

Rafael

[mcgyvr]

In the drawing model browser find the part and right click and select "properties" then uncheck "By layer" and select "Dashed" for the linetype.

You can also turn your selection filter to "Select Part Priority" and then right click on it on the drawing and do the same thing..

[DSSmithA5SDN · Accepted solution]

Maybe this will help but you have to find the part in the view that you want, then right click, and select hidden lines.

[blair]

You could select each line of the item and change it's line type. .I thought this had surfaced before and someone had a iLogic form to do this. You could search this forum for a similar post and see if you can find the iLogic code/form 

[rcolon9E4ZX]

I am looking to have a part display as hidden lines, AND be visible on top of all other model data. The part is hidden behind another, so I don't currently see any lines.

[mcgyvr]

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@rcolon9E4ZX wrote:

I am looking to have a part display as hidden lines, AND be visible on top of all other model data. The part is hidden behind another, so I don't currently see any lines.

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Then use the process DSSmith mentioned above.. Thats what that is for..

[rcolon9E4ZX]

When I implement DSSmith's process, I get this form

After clicking yes, the entire view is set to hidden lines. This is undesirable. I still want all hidden lines removed, EXCEPT for those in the part in question.

[rcolon9E4ZX]

My apologies. The view was in raster state for quite some time, and would be hidden lines were displayed as continuous with a thinner linetype, which at the moment made me believe all hidden lines would propagate. Yes, following DSSmith's process provides the desired functionality.

Thanks.

[rhasell]

Hi

There is an Inventor quirk, every now and again, after changing the line style of one part, the entire view changes to hidden line display = on.

You then have to switch off hidden line display for the view, and then do the individual part a second time. It always works the second time round.

Also, a tip for easy selection parts (If you can see them of course) is the use the "SHIFT-RMB" and select "Part Priority" don't forget to change back to "Edge Priority"

[Anonymous]

Thank you! this has been bugging me for YEARS!

What a ridiculous bug.