Deleting group lines

[JS34]

Hello-

I am very new to NX and I have a few questions that I hope people will share some information with me about

1. I've been trying to copy a sketch from one model into another model and I haven't been able to get it right. I want to copy the sketch curves from from one model and paste it in another.

2. Since I couldn't figure out how to copy and paste the sketch, I then tried to "edit with rollback" (of the sketch) but I couldn't delete the lines because they were part of a group.

I'm trying to avoid creating an entire new part by doing one of the above two. Not sure what to do but I would love to learn how to do the above. I'm using nx5.

Thanks in advance!!

 

[JohnRBaker]

Using NX 5.0 there is no problem copying and pasting the ENTIRE Sketch from one part file to another.

What you do is select the Sketch object, but NOT while you're in the Sketch task (i.e., edit with/rollback), either from the screen or from the Part Navigator, press MB3 and select the 'Copy' option.

Now open that other part file and go to the Main toolbar, select the 'Paste' icon (or go to Edit -> Paste...) and you you will be asked to select a plane of reference to place the Sketch object on.

Now if your desire is to only copy a few of the curves of an existing Sketch, while you can do that by simply selecting them (you will need to use QuickPick to select only the individual curves rather than the entire Sketch), pressing MB3 and selecting the 'Copy' option, when you 'Paste' these curves into a new part file they will NOT be part of a sketch but only standalone non-parametric curves without any constraints or dimensions (note that you can copy & paste PORTIONS of a Sketch, while retaining the constraints and dimensions associated with the curves selected, using NX 7.5).

Anyway, I hope this helps get you started. If you have any other questions, please feel free...

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

 

[JS34]

John,

I think I did something similiar today but the sketch curves were placed above the model I was working in. I tried constraining the sketch to my desired plane but nothing happened. I'm not sure why but the sketch wouldn't move once it was in the model.

I'll try that out tomorrow but do you have any ideas why I couldn't constrain the sketch curves within the model I pasted it in?

So I tried just deleting the lines within the sketch but I'm assuming group lines cannot be deleted.

Thanks!!

 

[JohnRBaker]

First off, a Sketch is NOT a 'group', however the curves are members of the Sketch object and will be selectd when the Sketch is selected. However, using QuickPick, the 3 dots (...) which appears near your cursor, you can select individual curves of a Sketch and delete them. Just place your cursor over the Sketch curve you wish to delete, wait until the 3 dots (...) appear and then push MB1. You'll get a dialog showing all of the objects which you can select, in this case, the Sketch itself AND the curve which your cursor was over. Just select the curve from the list, and hit the Delete button. Now you may get a message telling you that some associated objects may also be deleted, but if after accepting this message, if the results turn out to be NOT what you expected, you can always perform an Undo and return the model to where it was before you deleted the sketch curve.

Now as for moving/attachiong your Sketch to a different reference plane, while in the Sketch task (edit with/Rollback) go to...

Tools -> Reattach...

...where you will be given the opportunity to select a new Sketch plane and/or new orientation references.

Again, I hope this helps.

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