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NX10 drafting issues

Valued Contributor
Valued Contributor

We just upgraded to NX10 from NX8.5. I knew of some the potential issues brought on to the drafting by the new dimensioning function. I had been in those famous webinars, but having not used it I was hoping it was not going to be that bad. But seeing is believing.

 

On the subjective side, I still do not like it. Any time you want to do something that not is right in the pop-up you have to wade thru an even longer menu - where the previous graphic interface has been removed, and to make things worse most of the stuff has been split up (so you find less function per menu entry).

 

On the less subjective side, I found after very little use that some issue are plain unsolvable. I had instances where I could not re-associate center lines, or dims. (the dim. would just stay as is regardless of new object selected, or some snap options would be simply not available, e.g 2-curve inters.). Yes, in older versions you would also at times be better off deleting & creating from scratch than editing, but I was hoping this has finally been fixed...

 

So now to 2 of my more specific issues:

  1. how do I add a new dim./location to a chain dim. ? (nx8.5 you could select the chain dim and click add...)
  2. how can I make the diameter dim. in the below left look like on the right ?

 dia'sdia's

 

Dan Iorga
Sulzer Pumps US
7 REPLIES

Re: NX10 drafting issues

Siemens Phenom Siemens Phenom
Siemens Phenom
For the chain dimension, open the Linear Dimension command and under the block titled "Dimension Set" set the Method to Chain and underneath select "Select Object". Select the existing chain dimension and then select the object you want to dimension to.

Regards, Ben

Re: NX10 drafting issues

Siemens Phenom Siemens Phenom
Siemens Phenom

For the Radial dimension, is this the icon/option you're looking for "Radius to Center"?  Edit the dimension, drag the value where you need it and use the on-screen toolbar to select the option:

 

radius to center.png

 

Regards, Ben

Re: NX10 drafting issues

Phenom
Phenom

For #2 (assuming a diametral dimension), double click on the dimension and toggle the "arrows out" option (in the bottom row of icons on the pop-up dialog) and drag the dimension to the desired location.

Re: NX10 drafting issues

Siemens Genius Siemens Genius
Siemens Genius

I see Ben replied to the chain dimension ,

 the second question, is it that you want the text to be on the left side of the arc center and not extend to the invisible side of the arc ?

 

Are you trying to dictate to NX what dimension type you want or are you using the "radial" dimension, or the "Rapid dimension + inferred" ?

 

I get the solution seen in the right image by default.

 

Regards,

 Tomas
 

Re: NX10 drafting issues

Valued Contributor
Valued Contributor

For #2 -> cowski got the right anser. Seems that was 1 option I had not tried, as I was only using the full menu to tweak stuff. Thanks !

 

When it comes to #1 -> still no solution. The solution suggested by Ben does not seem to work (here ?). The dims are already part of a shain, so my edit menu (which only applies to 1 dim at a time) looks like this - no option to set the Method to Chain and underneath select "Select Object".

 

chain.png

Dan Iorga
Sulzer Pumps US

Re: NX10 drafting issues

Siemens Legend Siemens Legend
Siemens Legend

Here is a link to information that demonstrates how to edit a baseline dimension:

https://docs.plm.automation.siemens.com/tdoc/nx/11/nx_help/#uid:xid1128417:index_drafting:id701707:i...

 

This approach should also work for a chain dimension. Maybe there was some step in the procedure that you didn't originally follow?

Re: NX10 drafting issues

Valued Contributor
Valued Contributor

OK, that was it. You cannot go in edit mode the normal way (dbl-click), you have go specifically thru that sequence in order to be able to now add a new dim/location. (the sequence: dry open the Linear Dimension command and under the block titled "Dimension Set" set the Method to Chain and underneath select "Select Object". )

 

Anyone thinking this is an improvement doesn't use NX much...

Dan Iorga
Sulzer Pumps US