Some edges do not display in drawing

[gchampoux]

In one of our assembly drawings, some models edges are not displayed (that should definately be displayed).

We saw this many years ago, and thought it was fixed, but it seems to have returned.

It happens when some parts of the assembly interfere, but not by a noticable amount.
If we blank the suspect interfering part, the all edges of the rest of the assembly displays correctly.

The missing edges can happen anywhere, and not neccesairily near the region of interfereance.
Sometimes, it is the outermost edges of a part, which really looks wierd.

Has anyone else see this behavior?

CE Pro 5 M150 with Windchill Intralink 9.1 M060

Gerry Champoux
Williams International
Walled Lake, MI

[TomU]

Yes, we are seeing this with WF5 (CEP) M120 as well.

[DarrinHiebert]

Hummm…



I thought that it was always this way, and has been for quite a while.



This is one thing that we use to check for interference. Not that it’s a
golden rule, but sometimes when you see things that are not “right”, you go
back and you look at it under a microscope, and you find out that they are
interfering. For us, though, we never SHOULD have parts that interfere. We
do run anything here that would be an interference type fit, so for us, this
has always worked out good…

[justgeo]

Wildfire 3 here, same troubles.

We work in sheetmetal so it happens frequently. Most often when running a post through a s/s countertop. The laser cuts the hole undersized so there is supposed to some interference between the parts. Once the break operators bump the hole it grows to the right diameter for the post to fit. The disappearing lines play havoc with our drawings so we often resort to cutting a channel in the pipes or adding the missing lines in the drawing. Neither solution is ideal but it gets us by.

If you find out another way please let us all know.

Justin Giaquinto
Engineer | BSI, LLC

Direct 303.331.8777 | Ext. 341
Phone 1.800.662.9595
Fax 303.331.8444
Mail BSI, LLC | 5125 Race Court | Denver, CO 80216
Web www.BSIdesigns.com
back and you look at it under a microscope, and you find out that they are
interfering. For us, though, we never SHOULD have parts that interfere. We
do run anything here that would be an interference type fit, so for us, this
has always worked out good...

[jeffsampson]

body{font-family: Geneva,Arial,Helvetica,sans-serif;font-size:9pt;background-color: #ffffff;color: black;}Gerry,

What you describe is (mostly) intended functionality. We have the setting "no hidden lines" to hide any lines that are not an exposed edge, and that's exactly what Pro does when a press fit shaft is inserted into it's hole. Though small, there IS an interference and so Pro hides the edge because technically it is not exposed. Annoying? yes, but proper functionality. As others mentioned, you can add a very small cut to either part to create an exposed edge that will show up in the drawing

As to your claim of it doing this when there is NOT an interference, I'm not sure what is going on there. That shouldn't happen.

Best regards,

Jeff

--
Jeff Sampson Engineering
-

[TomU]

Jeff,

Not sure exactly what Gerry is seeing, but when it occurs here, probably half the model disappears in the drawing, not just the area where the (extremely small) interference is occurring.

Tom U.

[gchampoux]

Thanks to all that replied.

Along with your responses and some more searching at PTC's knowledgebase, I have confirmed that this is indeed a situation where there are interfering assembly parts (such as a press fit). PTC says that this is still a known limitation of Pro/E, and they do not intend to address it because it would introduce severe performance penalties.
The only adequate work-around is that we must ensure that parts do not interefere.

Gerry Champoux
Williams International
Walled Lke, MI

In Reply to Gerry Champoux:

In one of our assembly drawings, some models edges are not displayed (that should definately be displayed).

We saw this many years ago, and thought it was fixed, but it seems to have returned.

It happens when some parts of the assembly interfere, but not by a noticable amount.
If we blank the suspect interfering part, the all edges of the rest of the assembly displays correctly.

The missing edges can happen anywhere, and not neccesairily near the region of interfereance.
Sometimes, it is the outermost edges of a part, which really looks wierd.

Has anyone else see this behavior?

CE Pro 5 M150 with Windchill Intralink 9.1 M060

[DarrinHiebert]

I remember that happening in an earlier revision as well, but don’t recall
which one it was. Like Gerry said, it was MANY years ago, though that this
happened…

[#9]

I’ve seen it recently (WF4? 5?).



Gerry,

When exactly are you seeing this? On screen? When sending to plotter? MS Print Manager? Publish to PDF?



Have you tried adjusting the Quality? (i.e. overlap check?)



~Dan

[TomU]

WF5 M120. Visible on screen in drawing mode. Never tried to print with it showing. It almost acts like part of the model is no longer there. I can’t remember for sure, but I think it may have only happened when the view display was set to hidden line in the drawing. Eliminate the interference (again, extremely small) and everything becomes visible again.

Tom U.

[DarrinHiebert]

What you’re describing here is very much like the “intended” functionality
that Jeff was talking about in his earlier reply.



It will only show up in hidden line mode, IIRC…

[jwagh]

I don't intent to bring up a ghost thread, but what about an assembly where a screw is going into a threaded hole. For example, a #8 screw, with a nominal thread dia of .164 goes into a hole feature using UNC table, threaded for a #8 is .136. There is an interference in the assembly. In the ISO view, the hole disappears and the lines for the shaft of the screw. Any tips, tricks or solutions we can use?

Thanks!

[cprice]

I have been thinking about the interferences a lot lately. How about changing one of the interfering parts into a Flexible Part within the assembly?

You could then reduce the offending component to a size that would eliminate the interference in that particular assembly. This would eliminate the hidden line problem in the drawing.

Just pondering the idea.

[jwagh]

Interesting, but it won't work if you set your models to READ ONLY before releasing it.

[llokesh]

DRAWING VIEW- VIEW DISPLAY- DISPLAY STYLE (SET TO HIDDEN)-CLOSE

LAYOUT- EDGE DISPLAY- HIDDEN LINE(IF HIDDEN)- SELECT THE EDGES WHICH ARE NOT VISIBLE- OK

GO BACK TO..

DRAWING VIEW- VIEW DISPLAY- DISPLAY STYLE (SET TO NO HIDDEN)-CLOSE

YOU WILL FIND THE HIDDEN EDGES THAT YOU HAVE SELECTED.

THANKS