Drafting: Center Mark size (how to set for a drawing) 2

[potrero]

NX6.0.1.5 MP2

When creating a drawing with holes and Center Marks enabled, sometimes the Center Mark size is larger than desired. The size can be altered for an individual Center Mark by either double-clicking it, or right clicking it and Editing the Gap, Center Cross, and Extension. You can inherit the size settings from another Center Mark as well.

My question is: how would you resize ALL Center Marks in a drawing (and there might be a LOT, so manually doing them one by one is very undesirable)?

I've tried selecting multiple Center Marks, but the Edit option disappears from the Right-Click menu if you've selected more than one Center Mark.

Thanks.

 

[JohnRBaker]

The best that you can do is to delete all of the existing ones and create (using the multiple points option) them over again with your desired settings, but only if you have no more than 100 holes that you try and select at one time.

There is a way to automatically do ALL the holes in an existing view, but it involves editing/selecting a new Drafting Standard in Customer Defaults and then reopening your drawing in a new session and then with the Drafting Preferences set to using the current standard (the one you edited/selected in customer defaults) as opposed to what the standard was that was assigned to the drawing template, you can then, after deleting the old centerline symbols, use the Automatic Centerline symbol function.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

It probably makes sense to put in an enhancement request to be able to edit multiple centre lines settings for that one as it does seem out of step with all the other presentation aspects that are simply edited under "style".

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[ufsure]

I have attached a UGopen program that will edit multiple center lines. When the selection dialog comes up either 'select all' or select individual center lines. Next, the dialog will display the current values of the first center line in the selection list. Enter new values and you should be done.

If you have any problems, please let me know.

Suresh
www.technisites.com.au

 

[jschetl9]

HI any one saw my simulation question please....
(In my previous post, I attached the drawing)
I am trying to apply vector force(unit force) at one end of the simulated 4-barlink mechanism. I used Revolute+Revolute+Universal and Ball joints at each end.
Grubler count is shwoing 0 and the dof also zero (with driver on one of the revolute joints).
Now when I apply unit vector force, when I run the for excel map the simulation is giving a torque of 0.9Lb-in where as the FBD free body diagram gives an end torque of 8.63Lb-in.
Pl guide.
Thanks
Srini

 

[potrero]

Srini,
Probably not a great idea to be spamming other threads about your question, since you've already posted about it elsewhere (thread561-239103), and people in that thread are trying to help you out...

 

[potrero]

Suresh,
Thanks for the code. Can you explain how to get it up and running? I see the .dll, but I'm not familiar with how to use this type of extended functionality...
Thanks.

 

[potrero]

Suresh,
Nevermind, I got it...

File > Execute > NX Open
or
Ctrl + U

This is great! How'd you make it?

 

[ewh]

Edit -> Style -> Symbol -> Detail Filtering -> Centerline -> OK -> OK -> Select All

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[ewh]

You need a sample centerline of the style that you want, then after doing the above, use "inherit" and pick your sample.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]