Show lines of thread in drawing

[Spedex]

Hey guys, i am using PTC Creo Parametric 7.0 (Student Edition)

I created a thread on a pin.

Unfortunately, it does not really show the outlines (actually the inner lines) of the thread:

My visibility option is on "only show visible edges / lines"
If I select "show also not visible edges / lines", creo will show the whole thread but also everything else, which is not good for me.

Can somebody help me with this problem?

Greetings,

Spedex

[kdirth]

You can use Edge Display in the edit section to control the visibility of lines.

• Select edge display
• Select view settings for line
• Select one or more lines (will highlight unshown lines as your curser passes over)
• Select OK

[Spedex]

What should i do now? I clicked on "Edge Display" and selected the hidden edge. But after pressing OK or Done, nothing changes.

[Spedex]

Video of it:

[Tdaugherty]

Take a look at this video. I think it explains what you're trying to do. 

https://www.youtube.com/watch?v=d4Pgo0Wt4FI 

[Spedex]

Hey, i already watched the video.

I followed the steps. I can definitely erase solid lines. But i fail trying to show the hidden thread lines.

Idk how long it takes for the video to be released, but you will see it there i think.

Edit: The video is now public.

[TomU]

@Tdaugherty,

I wonder if something else is going on here.  I'm not able to erase the silhouette edge of the cosmetic surface.  By default this should be visible anyway.  I'd really like to know what changed to have it not display in the first place.

[Tdaugherty]

@TomU 

I second that. I can erase other hidden lines but not the ones related to the cosmetic thread. I was wondering if maybe it had something to do with the hlr_for_quilts config option but I'm not sure. Still looking.

It does seem that a viable work around is to set the view display to hidden and then erase the non-quilt hidden lines. Basically just reverse the order of operations.

[Spedex]

Is there a way to make the thread line thinner?

Doesnt work with the "Line Style" option.

I click the thread line (the visible, vertical one) and change the thickness values for example to 0, but it stays as thick as before. It works with all the other lines. I can also not make this line not visible with the "Edge Display" option.

[kdirth]

Select "Hidden Line" in the menu first ( you have No Hidden selected), if you want a dashed hidden line, then select the line then OK.

[kdirth]

OK...  Cosmetic threads do not seem to follow the same rules.  I cannot show the silhouette edge in 4.0 using edge display.

[TomU]

Same here.  Tried Creo Parametric 6.0 and 7.0.  Can't seem to control individual edges of a cosmetic.  Either all of them show or none of them show.  I don't understand how @Spedex hid it in the first place.  We must be missing something...

[kdirth]

I believe he his view display is "No Hidden" to reduce hidden line clutter in the rest of the drawing.

[TomU]

Possibly, but 'no hidden' in my test drawing continues to show the cosmetic thread.  The thread only hides in the three shaded modes for me.

[Tdaugherty]

Hi, 

Is your part externally threaded or internally threaded? It's hard to tell from the screenshot. I would assume external based on the relief cut...???

How were the threads created? Are they actually modeled or did you use a cosmetic thread feature? If you used a cosmetic thread feature, you won't be able to see the threads. The cosmetic feature is just a surface. You'll be able to see the edges of the surfaces but nothing in the middle. 

How it looks in 3D:

How it looks in 2D:

View display settings for the drawing view:

I tell my guys to avoid 3D threads whenever possible due to their affect on performance. We use cosmetic thread features in applications like these. To call it out on the drawing, we just use a manual leader note (not the best method but it's quick). 

Ty

[Spedex]

I am using an external thread (cosmetic thread) and i dont see the edges, as you can tell from the picture.

[TomU]

Where is this visibility option you're talking about?  I'm not seeing anything with that name...

[Spedex]

I was using the german version of Creo. That's why it was hard to translate. Changed it to English now.

[MartinHanak]

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@Spedex wrote:

Hey guys, i am using PTC Creo Parametric 7.0 (Student Edition)

I created a thread on a pin.

Unfortunately, it does not really show the outlines (actually the inner lines) of the thread:

My visibility option is on "only show visible edges / lines"
If I select "show also not visible edges / lines", creo will show the whole thread but also everything else, which is not good for me.

Can somebody help me with this problem?

Greetings,

Spedex

---

Hi,

to hide cosmetic thread in specific drawing view:

• in model ... put cosmetic thread into new layer
• in drawing ... hide the layer in specific drawing view, only

[T_UFF]

You need to change the drawing option setting 'hlr_for_threads' to 'NO'