Driving Dimensions

[KLineDesign]

One other one that may tie into my last thread.... How do I make dimensions on the drafting side 'driving dimensions'? I see the option under edit, but I can't get it to work. (I may never use it, but I thought this could be part of getting tolerances in sketch to be the same dimensions and tolerances in drafting. Could be part of PMI too, I don't know)

Thanks for your time,
KLINE

 

[joycejo]

Sounds like you have used Pro/e in the past.

In NX you can do this if you follow a couple of rules.
First you need to set the environmental variable UGII_DRAFT_EXPRESSIONS_OK to 1
Next you need to add the feature parameters of the sketch to the selected view.

Now when you have the tool – expressions dialog open and pick one of the dimensions inherited from the sketch the associated expression will highlight on the expression list. You can change the value of the expression and update the model from drafting.


John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO

http://www.myigetit.com

NX5,6 Solid Works, Solid Edge

 

[Xwheelguy]

I thought you also had to create a reference set for the sketches to go into, then show the reference set on the drawing, or something to that effect. I never practiced this workflow, just investigated how it was done.

I didn't care for it because if you sketch a cylindrical or conical shape, you have to sketch the entire diametric profile, not just half of it in order to get the diameter dimensions to show up correctly on the drawing.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[KLineDesign]

All these steps must be done to make the last button in the attached image available?

Let me know,
thanks,
KLINE

 

[Xwheelguy]

KLINE,

I don't have the resources available to completely answer your question, however this should be outlined in the Documentation in the Sketcher or Drafting sections.

When I ran a test on using this capability, I do remember having to create a single component assembly, then adding the entire sketch to a reference set in order for the sketch dimensions to appear in the drafting view as well as drive the model from the drawing.

Like I stated before, I felt that I was doubling the work in my sketches (because most were revolved sections, which required I sketch both halves and make one side all reference curves) just to get diameter dimensions to appear as diameters rather than radial dimensions (dimensioning half of the revolved profile) on the drawing view(s).

Another issue I had with this workflow was that you don't get to see what all is affected with the model right away. If you have sketches constrained to one another in modeling, you might not see the change when editing a driven value in Drafting via the drawing.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[KLineDesign]

Thanks Tim, I was unable to find any documentation about the driving dimensions. I agree that it is mostly a poor practice, but has it's uses (tabulated parts could be nice)...I prefer to keep much of design intent captured in sketches, and editing a single dimension out of context of the sketch (or model for that matter) could be an issue. The revolved situation also changes this, but could be worked around.

I was looking into this for the ability to have the same dimension as sketched shown on the drawing. I don't need it to be driving the model; I thought possibly 'driving dimensions' would bring forth the actual sketch dimensions with tolerances and that is my goal.

I think I'll load up NX7 today, and that will cure all this!

Thanks for your replies,
KLINE

 

[Xwheelguy]

KLINE,

That's exactly what happens. The sketch dimensions will appear on the drawing. You create a sketch to be used in the model. You perform various steps to prepare the model so that the sketch dimensions can be used on the drawing (these will drive the sketches, which in turn drive the model). Once you have the model and such ready, you place your view on the drawing, and the sketch dimensions should show up on that view. All of this is a very generic description for the actual steps. I don't have a seat of NX in front of me to go through each step one by one.

What you need to search for in the NX Docs is Inherit Sketch dimensions. I couldn't remember the keyword yesterday when I left my last response. Do a search on that and see what you find. It should be the process I've described above (make Modeling sketches, use sketches to create solid model, put sketches in reference set, add model as component of new assembly part file which will be the drawing, go into Drafting and add views and use Inherit Sketch Dimensions command). Once you've got that all done, you'll be able to edit the model via the drawing like John Joyce & I have described in our posts.

Incidentally, driving dimensions in NX are usually defined as Drafting Sketch dimensions, which are completely different than those in the Modeling Sketcher. Didn't want to get things mixed up between Drafting sketches and Modeling sketches.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[KLineDesign]

Tim, it appears that I have to wait for PMI to be here or NX7.5 maybe. See, the sketch dimensions inherit alright, but the tolerances do not. I can get tolerances to show up, but they are not as specified in the sketch (even though the 'use sketch dimension style' button is selected the values of the tolerances keep defaulting to .005). It may be true that I have to do something else to get this to work, but I will only use it if it is as simple as it sounds like it will be in NX7.5.

Also, thanks for pointing out that the "Driving Dimensions" are drafting sketch dimensions! That would've pretty much eliminated this thread.

Thanks everyone,
KLINE

 

[Xwheelguy]

KLINE,

In order to get tolerances to show up, you might have to right click on the dimension shown on the drawing while you are in Drafting (NOT in the Modeling Sketch environment or Drafting Sketcher) and choose Style or one of the other dimension-related commands on the MB3 pulldown menu. I would be shocked if tolerances were not supported in the Inherit Sketch dimension workflow.

Another option would be to call GTAC and have them walk you through it, if your maintenance is current.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[KLineDesign]

I am leaning towards them not being currently supported in NX6. They do indeed show up, just not correctly (as specified in the Sketch). Again, I am looking to specify some of the tolerances while designing....and then later down the road inherit them while detailing.

 

[Xwheelguy]

KLINE,

I wouldn't be surprised if you run into obstacles when trying to apply tolerances to a Sketch in Modeling. I would recommend trying to complete the Sketches without them first to see if Inherit works like you expect. You can then go back and edit the dimension Style to see if you have any luck with getting tolerances to show up. I would do that part in Drafting and not within the Modeling Sketch.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[edgray]

This is slightly off the this thread but in reply number 3 NKwheelguy mentions the need to sketch the both sides of the revolved profile to get the diameter dimension in the drawing. I do this by sketching a reference line with a midpoint constraint on the revolve axis and constrained to the profile on one end. I then dimension the reference line with the diameter value. I do not know if this will work when using the sketch in the drawing, we don't use that function. It is very handy when I want to control a diameter dimension at a certain depth in a part with draft. In the drawing the depth dimension could be the basic dimension for the measurement location in the GD&T.