Creo Drawing, Show/Erase threads

jskraba · ‎May 14, 2014

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.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

MikeBrattoli · ‎May 14, 2014

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

[Description: Description: New Moen Logo.tif]
[Description: Description: Description: Description: Description: Description: Description: Description: fb]<">http://www.facebook.com/moen> [Description: Description: Description: Description: Description: Description: Description: Description: Description: t_logo-a.png] <">http://www.twitter.com/moen> [Description: Description: Description: Description: Description: Description: Description: Description: YouTube] <">http://www.youtube.com/moenfaucets> [Description: Description: Description: Description: Description: Description:

DonSenchuk · ‎May 14, 2014

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.

StephenW · ‎May 14, 2014

Select the view, right click "erase cosmetics".

One thing they made easier in Creo2.

MikeBrattoli · ‎May 14, 2014

Thanks Steve - never even checked the RMB menu

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

nrollins · ‎May 14, 2014

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...

drichards · ‎May 14, 2014

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.

MIchael_Ohlrich · ‎May 14, 2014

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

[cid:image001.jpg@01CF6F58.633E0D90]
www.benchmade.com<">http://www.benchmade.com>

CONFIDENTIALITY NOTICE: This e-mail communication and any attachments may contain confidential and privileged information for the use of the designated recipients. If you are not the intended recipient, (or authorized to receive for the recipient) you are hereby notified that you have received this communication in error and that any review, disclosure, dissemination, distribution or copying of it or its contents is prohibited. If you have received this communication in error, please destroy all copies of this communication and any attachments and contact the sender by reply e-mail or telephone (503) 655-6004).

mlocascio · ‎May 14, 2014

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

drichards · ‎May 17, 2014

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.

jskraba · ‎Aug 29, 2014

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?

tallen · ‎Aug 18, 2015

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

jskraba · ‎Feb 17, 2016

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.