Appended text in drafting
Appended text in drafting
(OP)
thread561-294129: Cannot edit appended text in Drafting
I am having the same problem that was stated in this thread. I created sketch lines in drafting that I then dimensioned and if I try to change the text of the actual dimension it simply snaps back to what it was. Wondering if anyone has a solution to this.
I am having the same problem that was stated in this thread. I created sketch lines in drafting that I then dimensioned and if I try to change the text of the actual dimension it simply snaps back to what it was. Wondering if anyone has a solution to this.
Sam Slivinski
Using NX 6
Manufacturing/Aerospace





RE: Appended text in drafting
The easy answer is: don't use a sketch line.
My guess is, it is a bug with sketch lines. The dimension you place automatically becomes a driving dimension (sketch dimension); but even if you turn off the "driving dimension" option, the dimension text cannot be changed manually.
You may have to customize your drafting environment to add the line command, but when you create a non-sketch line and dimension it, the dimension text can be changed manually.
www.nxjournaling.com
RE: Appended text in drafting
www.nxjournaling.com
RE: Appended text in drafting
Not saying I agree with it or that you're wrong, but according to IR# 1894281, that's GTAC's response to your query.
Tim Flater
NX Designer
NX 7.5.4.4 MP8
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Appended text in drafting
Thanks for the IR number & explanation. That makes good sense that you cannot change a sketch dimension.
Herein lies the problem. After creating the sketch line and exiting the sketch, if you dimension it (using the "true drafting dimension" command) the dimension created is a sketch dimension. I see no way to create a "drafting" dimension on a sketch object created in the drafting environment. User beware, the object you dimension determines the type of dimension you get.
www.nxjournaling.com
RE: Appended text in drafting
It might be a decent idea for an ER to allow for dimensions to have a toggle (drive geometry toggle) to allow for scenarios like this. I believe CATIA v5 has something like this - I could be mistaken about that though; it's been a while since I poked around with v5.
Tim Flater
NX Designer
NX 7.5.4.4 MP8
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Appended text in drafting
Sam Slivinski
Using NX 6
Manufacturing/Aerospace
RE: Appended text in drafting
Sam Slivinski
Using NX 6
Manufacturing/Aerospace
RE: Appended text in drafting
Or use a line instead of a sketch line as suggested in my first post.
www.nxjournaling.com
RE: Appended text in drafting
Sam Slivinski
Using NX 6
Manufacturing/Aerospace
RE: Appended text in drafting
If you have strong feelings about allowing the sketch dims to have the ability for their values to be manually edited, call GTAC and give them that IR number, have them attach your contact info to it and then turn around and put in an ER. It won't do any harm....at least it might give their developers something to ponder, especially if in fact a competitor's software has this feature built into it.
Tim Flater
NX Designer
NX 7.5.4.4 MP8
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Appended text in drafting
I hope this helps.
RE: Appended text in drafting
Have you then tried to edit the dimension text after toggling off the "driving dimension" option? I suggest you try.
(this was referenced in my first post on 29 Nov 12 9:32)
www.nxjournaling.com
RE: Appended text in drafting
RE: Appended text in drafting
www.nxjournaling.com
RE: Appended text in drafting
RE: Appended text in drafting
What steps are you taking for a successful edit?
www.nxjournaling.com
RE: Appended text in drafting
Sam Slivinski
Using NX 6
Manufacturing/Aerospace
RE: Appended text in drafting
1. Insert a sketch line
2. Insert->Dimension->Inferred
3. Select the sketch line and then toggle off driving dimension
4. Edit->Annotation->Text
5. Select the dimension
6. Change the value (note at this point you get the dialog box asking you to confirm what you are doing)
7. Select 'OK' on the dialog box (the value is changed on the dimension)
8. Press close on the dialog
At what point are you seeing the value reverting back to the original value?
RE: Appended text in drafting
Your method does indeed work, thanks for sharing.
www.nxjournaling.com
RE: Appended text in drafting
RE: Appended text in drafting
www.nxjournaling.com
RE: Appended text in drafting
There is some logic to it, even if not obvious. A "Sketch" dimension can be toggled back and forth Reference / driving whilst a "Drafting" dimension can never become (?) a sketch constraint. When creating the dimension as noted by Mreleven, the resultant dimension is a "drafting" dimension.
- run the example as described, then create another dimension as i assume that Cowski did, ( first place as driving, then RMB Convert to reference)
Then , when these two are in place, information -object and select both + OK. The "Sketcher" dimension will have notes about "Parent Sketch" and "Driving Expression" whilst the other dimension does not.
The question is if one can convert the "sketcher dimension" to become an "drafting dim".
Regards,
Tomas
RE: Appended text in drafting
RE: Appended text in drafting
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:
To an Engineer, the glass is twice as big as it needs to be.
RE: Appended text in drafting
Sam Slivinski
Using NX 6
Manufacturing/Aerospace