Show Removed Portion On DWG (IDW)

[gobluejd]

I have a part (for simple explination 1/4" Bar Stock 8" Long x 1.5" Wide).  We need to modify it and remove say 1" (Final is 7" x 1.5").  I need to show the proccess in a drawing.  So I need to show the FULL PIECE prior to the cut and then a dotted line showing where to remove the 1".  Obviously I bring the "cut part" into a IDW but I can not show the part that was removed.  Hope this makes sense.

Thougths? I attaced a AutoCad file showing what I mean. 

[JDMather]

Investigate Overlay views.

[gobluejd]

That appears to be for assemblies? This is a PART and not in an assembly.

[wimann · Accepted solution]

I mean... I feel like there are a couple of approaches. I don't do this very often so I haven't yet found the "best" way for me. You could maybe place a workpoint on the face before the cut then project that point into your .idw and use it to fully constrain a sketch? There aren't many ways to show a part pre-cut and cut in the same view with the same part. You could derive it to show before and after. You could just sketch the profile that is to be cut away (not really the best unless you have some sort of reference like the workpoint I mentioned before).

Any of this help? Other questions? Perhaps pertaining to the things I've just mentioned?

[brendan.henderson]

Placing the stock bar part into an assy and converting the assy to a Weldment gives you extra functionailty when it comes to the drawing (machining). You don't have to place any welds. Probably not the overlay dotted line you're after but maybe useable.

[SBix26 · Accepted solution]

I use multi-body solids to do this.  In the attached example I modeled the as-received part (vendor does not have models available), then split it into two solids.  In the drawing, I placed views of the part, then selected the "removed" solid in each view and changed linestyle to phantom.  Not too difficult, at least in this case.

For the part's use in assemblies, I created a view (named "Trimmed") with the removed solid's visibility turned off, and used this when placing the part.  This is not a perfect solution, though, since I suspect that the invisible solid would still contribute to mass calculations; Make Component might have to be used to derive the remaining solid into its own part.

Sam B

Inventor Professional 2015 SP1 Update 1
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

[gobluejd]

Exactly what I was looking for!!! Thanks to all that commented.