Tolerances in Sketch, is it worth it?

[KLineDesign]

Just looking for some opinions on a Design Intent idea. I have never included tolerances in sketch dimensions, but I thought maybe it would be nice in capturing design intent and furthermore it would be cool if it automatically showed while annotating...

Just an idea, do you think it would be worth it?

KLINE

 

[joycejo]

Have you tried this to see how it works?

I did and the tolerance from the sketch does not inherit onto the drawing. I see no advantage to adding the tolerance onto the sketch. I would change the dimension style on the drawing and add the tolerance there.

John Joyce
Tata Technologies
1675 Larimer St.
Denver, CO

http://www.myigetit.com

NX5,6 Solid Works, Solid Edge

 

[KLineDesign]

You're correct the tolerance does not inherit onto the drawing. That is idea...would it be worth it to have this happen (perhaps it already can, but I couldn't get it to work)? I kind of think it would be a nice feature because often I consider tolerances while sketching, and then have to revisit those same tolerances while detailing. If I could inherit the tolerance, or have it actually be both the sketch dimension and the drawing dimension I would only visit the tolerance once, plus I could see the tolerance in context of an assembly without having to look at the drawing.

I think this is worth an enhancement request (and once again, perhaps it is already there...tell me how if so!), anyone else think it is not?

Thanks for your time,
KLINE

 

[Jaydenn]

Have you looked at PMI(product and manufacturing information)?

You add the design critera to the model, not the sketch. Otherwise it will get you the same result.

Drop a view into a drawing, inherit PMI and voila... Drawing is detailed, tolerances and all.

I'm not sure what version PMI appeared in, but I use NX6 and it works there.

J

 

[JohnRBaker]

Well in NX 7.5 you can 'convert' (actually it's more like a 'clone') Sketch dimensions into PMI objects and in that case, any 'Style' changes applied to the Sketch Dimension, such as tolerances, will be properly moved from the Sketch to the PMI Dimension.

And if that wasn't cool enough, once you leave the Sketch task and you see that 'PMI Dimension' in your model, if you double-click on that Dimension, you'll be able to edit it (and the model will update) as if it were still a Sketch dimension (which in reality it actually is).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[rg006]

Hello,
Just a quick though on this. I have played around with "sketch to drawing" tolerances and dimensions before on another CAD system, and the problem I had was that you have to think ahead very well. Whatever dimensions you use on the sketch are the dimensions that you have to use in your drawing. So you have to be very aware of good dimensioning practices (ie. only dimension something ONCE and in its normal perp. view). IF you chose to use different dimensions in the drawing than you used in the sketch you have to be very careful with bonus tolerancing and on top of that you have to pay a lot of attention to you primary and secondary datums, at least more so than if you did all the tolerancing in the drawing. We are switching to NX6 soon ( I hope) and now I am rather jealous that we are not going to NX7.5 cause Johns comment was rather exciting (as far as an engineer can get excited...) but anyway, hoped this gave you some things to think about.
Thanks,
Rick

 

[KLineDesign]

Thanks for all the replies. I figured it was in there, or will be shortly (There had to be a reason why Sketch Dimensions gained all the style of Drawing Dimensions). We just received NX7, perhaps I'll load it right now. We currently don't have a PMI License, but next renewal hopefully we will do some trading in and up for the better.

Have a good weekend,
KLINE