Internal Sketcher for Holes- new point created upon editing dimension, NX9 1

[scope63]

Hi all

i am using NX9 and have found that when i use the Sketcher inside of the hole command with continuous auto dimensioning set to on i will get a point created- this is not the issue. when i double click the dimension to edit its position i get a brand new point created! why? is there a setting that i have missed to turn this on or off?

Scott Copeland

 

[JohnRBaker]

I was not able to reproduce this behavior using NX 9.0.3.4. You say that you're getting two points? How is this being determined? Are you getting some kind of error where multiple holes are being created at the same location, or is there some other problem that this is causing?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[scope63]

hi John

i am currently running 9.0.2.5

i have attached a movie showing this example. i have been using NX/Unigraphics since v15 and have not seen this before. this is the first time i'm using NX9 so i know there are a lot of new changes so maybe this is one i missed!

Scott Copeland

 

[scope63]

hi John

one more thing, you will notice that i did not edit the auto dimension dimension, i created a new dimension, this should delete the auto dimension and create a dimension that has an expression attached, as in NX8.5 and previous version.

Scott Copeland

 

[phillpd]

I believe you need to set the Point Dialog option to Inferred to avoid that.

NX 9.0.3.4
NX 10 (Testing)
Windows 7 64 (Windows 8.1 Tablet)

 

[JohnRBaker]

OK, I've verified that NX 9.0 and NX 10.0 is behaving as shown in your video, but not NX 8.5, so this is a regression. As phillpd has stated, if you use the 'Inferred' point method instead of 'Cursor Location' you only get a single point, so that should be your normal workflow. That being said, I'm going to open a PR since this is a regression even though it's not exactly critical since there is a workaround, however I think I can force the PR to be considered critical since it IS a regression, but I also suspect that it will only fixed in NX 10.0.

Now that we've got that out of the way, make sure that you've started to use 'Inferred' for your point option, but when you go to create your hole(s), try NOT selecting the 'Sketch Section' icon from the Hole dialog but rather just pick the face that you wish to place the hole, near where you want the hole to be. This way you'll automatically be placed in the Sketch task AND your first Point will have already been created. This will save you several button clicks/icon selections. In fact, if you're only going to place a single hole and you don't mess with the dimensions, it only takes TWO button pushes, 'Specify Point' (AKA Select Face) and 'Finish' Sketch, versus FIVE using your workflow.


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[scope63]

oh good then i'm not doing something wrong!!
well since there is a work around i will do as suggested. thanks for your help.
i will wait to see if this goes into the next update or patch!

Scott Copeland

 

[JohnRBaker]

OK, I opened the PR and I just got word back that yes indeed, this was an issue in NX 9.0 and that it had already been resolved. The fix should be in the second NX 10.0 MR which should be available by the end of July.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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