Appended text in drafting 3

[SamSlivinski]

thread561-294129

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

 

[cowski]

Wondering if anyone has a solution to this.

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

 

[cowski]

Also, you may want to take this up with GTAC to see if this is "working as designed".

www.nxjournaling.com

 

[Xwheelguy]

Don't use sketch dimensions for things like this - they are intended to drive the sketch geometry, not have their values modified to "manual" values like true Drafting dimensions. This will occur even when you make the sketch dim reference. It's working as intended.

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

 

[cowski]

Tim,
Thanks for the IR number & explanation. That makes good sense that you cannot change a sketch dimension.

Don't use sketch dimensions for things like this

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

 

[Xwheelguy]

To be a little more precise with my previous posting, I should say that it's not a good idea to dimension to drafting sketch geometry if the intent is to have manual dimension text. View Dependent geometry or even a model-based sketch might be in order (if a sketch is absolutely necessary).

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

 

[SamSlivinski]

Thank you guys for the responses. So pretty much the answer is that I need to find away around using the dimension on the sketch lines?. Maybe I will try to make another view active then dimensioning it.

Sam Slivinski
Using NX 6
Manufacturing/Aerospace

 

[SamSlivinski]

The problem persists even when the view with the sketch in it is not active.

Sam Slivinski
Using NX 6
Manufacturing/Aerospace

 

[cowski]

So pretty much the answer is that I need to find away around using the dimension on the sketch lines?

Or use a line instead of a sketch line as suggested in my first post.

www.nxjournaling.com

 

[SamSlivinski]

Your solution does work, although I wish there was a less "sketchy" (no pun intended) way to go about it.

Sam Slivinski
Using NX 6
Manufacturing/Aerospace

 

[Xwheelguy]

Back in the day, that was the only way to go about it in Drafting - sketching in Drafting is relatively new to that particular application. I see the power of sketching in Drafting when you're making a 2D-only drawing. Mixing the sketches with model geometry in the views can get a bit dodgey, IMO, unless you're working with very, very simple parts that are almost entirely analytic-based geometry. It would be nice if I was able to see several different examples of how sketches can be used in Drafting other than the workflows I've used in the past.

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

 

[MrEleven]

In case you haven't contacted GTAC yet then I think there is an easy solution to your issue. The dimension commands have a "Driving" group on them with a button in it. After you select the geometry for the dimension the button will become sensitive. The initial state of the button is dependent on the geometry you select, if you select sketch geometry then it will default to on, otherwise it will default to off. If you do not want a sketch dimension then you can toggle the button off and you will get a non-driving dimension (a drafting dimension).

I hope this helps.

 

[cowski]

MrEleven,
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

 

[MrEleven]

Yes, I tried it and it worked just fine .

 

[cowski]

Great news! perhaps it has been fixed. What version of NX are you using?

www.nxjournaling.com

 

[MrEleven]

I tested against NX6. Perhaps it has regressed since then? What release (exactly) are you using?

 

[cowski]

I tested it on NX 8.0.3.4 and could not get it to work. Even after toggling off the "driving dimension" option, any attempt to edit the dimension text (Edit -> annotation -> text) would end with the dimension text reverting to the measured value. Doing an "info object" on the dimension shows that while it is not a driving dimension, it is still linked to an expression value.

What steps are you taking for a successful edit?

www.nxjournaling.com

 

[SamSlivinski]

I am on NX 6 and that is the what I attempted at first but it does not work.

Sam Slivinski
Using NX 6
Manufacturing/Aerospace

 

[MrEleven]

I am very perplexed. Here was the steps I took (basic I know, so if there is something I am missing then let me know).
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?

 

[cowski]

Seems I differed at step 3. I was selecting the sketch line and placing the dimension; step 3b was then to right click on the dimension, choose edit, and untoggle the "driving" option before attempting to edit the text. This apparently results in a sketch reference dimension rather than a drafting dimension.

Your method does indeed work, thanks for sharing.

www.nxjournaling.com