topic Creo Drawing, Show/Erase threads in 3D Part & Assembly Design

Creo Drawing, Show/Erase threads

jskraba — Sun, 13 Dec 2020 10:36:07 GMT

In WF3 there used to be option on Show/Erase popup for erasing cosmetic threads from the view. Where has this option gone in Creo 2? Namely, I have cross section view with some hidden edges shown and there are cosmetic threads I would like to hide from the view. How can this be achieved?Thanks

Creo Drawing, Show/Erase threads

MikeBrattoli — Wed, 14 May 2014 13:01:44 GMT

Jurij,

This will seem counter-productive but you can turn off the display of a cosmetic thread in the View Properties. Go to the View Display area for the view in question and check the "Yes" radio button for Hidden line removal for quilts - that will turn off the cosmetic thread in that view for "NON cross-section views". I have yet to find a configuration option that does this with Creo 2.0

Turning off the cosmetic threads for section views is more complicated.

[cid:image002.jpg@01CF6F53.20C69E50]

[cid:image009.png@01CF6F51.F4D61A60]

Make sure to select the "Yes" radio button for Hidden line removal for quilts BEFORE you make the view a section view.

Open the part or assembly that contains the cross-section. In your model tree, go to the Sections area (bottom of the model tree list). Select the desired section and choose Edit Definition to open the section dashboard.

[cid:image010.jpg@01CF6F53.20C69E50]

Go to the Options tab and pick the radio button "Include all quilts". When you go back to your drawing and update the sheet the cosmetic thread will turn off in the section view for that particular section but not in any other views, section or non-section

[cid:image011.png@01CF6F53.20C69E50]

[cid:image012.jpg@01CF6F53.20C69E50]

Makes total sense doesn't it :(!!!

Mike Brattoli
Moen Incorporated
Global Product Development Process Management
Administrator - PLM

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RE: Creo Drawing, Show/Erase threads

DonSenchuk — Wed, 14 May 2014 13:15:16 GMT

You could put them on a layer and hide the layer for those views.

In Reply to Jurij Skraba:

In WF3 there used to be option on Show/Erase popup for erasing cosmetic threads from the view. Where has this option gone in Creo 2? Namely, I have cross section view with some hidden edges shown and there are cosmetic threads I would like to hide from the view. How can this be achieved?

Thanks in advance.

Creo Drawing, Show/Erase threads

StephenW — Wed, 14 May 2014 13:22:24 GMT

Select the view, right click "erase cosmetics".

One thing they made easier in Creo2.

Creo Drawing, Show/Erase threads

MikeBrattoli — Wed, 14 May 2014 13:27:07 GMT

Thanks Steve - never even checked the RMB menu

Mike Brattoli
Moen Incorporated
Global Product Development Process Management
Administrator - PLM

Creo Drawing, Show/Erase threads

nrollins — Wed, 14 May 2014 13:41:14 GMT

RMB>"erase cosmetics"

This is the type of functionality I was requesting in my post on Sunday
evening asking for the good things about Creo. I know there is a lot to
complain about, but PTC has made improvements in some areas. The little
things add up to a lot. However, I have to laugh when I read propaganda
<

3. industry-leading user experience

Accelerate adoption and increase design efficiency. Access commands faster
with a

streamlined, customizable and familiar ribbon interface. State-of-the-art
tools such

as an intuitive 3D CoPilot, in-graphics toolbar and mini toolbars increase
design

efficiency. The new embedded command finder makes locating capabilities
faster

than ever. Faster installation and easy access to adoption aids - including
the new

LearningConnector, tutorials and Help resources - will get you up to speed
faster in

no time."

If anything comes to mind, please let me know. And sorry for hijacking this
post.

Thanks.

-Nate

RE: Creo Drawing, Show/Erase threads

drichards — Wed, 14 May 2014 16:20:01 GMT

As I recall this isone approach, they probably should already be on such a layer if admin is doing their job. Proper use and understandingof layers, their use and purposeappears to have been lost over the years.

Creo Drawing, Show/Erase threads

MIchael_Ohlrich — Wed, 14 May 2014 16:39:23 GMT

Nate - You can add that in assembly mode they added RMB for "repeat"!! Been waiting for this for years.

Just don't mention the measure utility... Hands-down the WORST "improvement" in CREO 2.0. I am not sure if they passed this off on some interns or something but, they definitely didn't use any competitor measure utilities before going off on this tangent. It was usable before but, not great and now it is horrible.

Michael Ohlrich, Design Engineer
Benchmade Knife Company
mohlrich@benchmade.com<">mailto:mohlrich@benchmade.com>
(503) 655-6004 x122

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Creo Drawing, Show/Erase threads

mlocascio — Wed, 14 May 2014 19:51:26 GMT

That does "work." The only problem now is that you don't have any
representation for the thread. For more complex assemblies it "may" be
advantageous not to show cosmetics. It's similar to the philosophy of not
showing the thickness of sheet metal parts.

Michael P. Locascio

RE: Creo Drawing, Show/Erase threads

drichards — Sat, 17 May 2014 15:24:24 GMT

The reason I believe the very best method of handling cosmetic threads is to have them on layers, is because their display can be handled in all subsequent drawings and models, all the way to the very top level, and it can be done all at once in one step. Showing/erasing them in the drawing where the threads are cut may often be the best method, especially if you want them to show in some views but not others. But several of the companies I've worked havemoved away from showing them as well as hiddenlines. So, it can be handled far more efficiently than hunting down each and every one of them to erase them.

RE: Creo Drawing, Show/Erase threads

jskraba — Fri, 29 Aug 2014 10:34:32 GMT

I found solution by myself and I would like to share it with others.

When on Annotate tab, select cosmetic thread you would like to hide (when dealing with cosmetic threads on pitch circle you should query or RMB select the right one, i.e. the one in the back), click RMB and select Erase. Kapooow -cosmetic thread disappears.

However, now I have another problem. I cannot find the way to get the erased cosmetic thread back. Any ideas?

Re: Creo Drawing, Show/Erase threads

tallen — Tue, 18 Aug 2015 16:02:33 GMT

The only way I have found, is to find the hole or cosmetic in the model tree, where you can then select Unerase. Really long winded, especially with a big model tree

Re: Creo Drawing, Show/Erase threads

jskraba — Wed, 17 Feb 2016 10:17:26 GMT

I have found out that when cosmetic thread is erased, there is an option Unerase cosmetic, however you need to select the view where you erased cosmetics immediately after Erase cosmetic command and then RMB click it. Unerase cosmetic command appears on RMB menu. This unerases all the cosmetics, that were erased.

Not exactly final solution but rather workaround, since you cannot directly select cosmetics, one or multiple, and unerase/erase them selectively.