Create diameter dimension in sketch? 1

[fighterpilot]

For the Pro/E users who've switched to UGNX5. Is it possible to make a diameter dimension in UG sketcher? In Pro/E you could drop a centerline, drop a sketch line parallel to it, click the centerline, click the line and then click the centerline again, creating a diameter dimension.

Thanks...

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

No, not in the sketcher. Create an expression for Diameter, and then dimension the half-profile (radius) and use the Diameter expression divided by 2.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[fighterpilot]

That's not really my intent but oh well. My intent is to drive by a diameter dimension in my sketch. Creating an expression is just another step that is not IMO, intuitive.

More brain retraining required.

--
Fighter Pilot
Manufacturing Engineer

 

[Xwheelguy]

fighter,

You could define your centerline (draw it, or use a Datum Axis that helps define the sketch), make it reference if you draw it, then mirror your sketch about that centerline and make the mirrored side reference curves as well. Just use horiz. or vert. dimensions and dimension between the 2 halves. We do this quite a bit designing wheels. Might be a bit more challenging if your centerline is not related to the Datums defining your 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.

 

[MCGNX]

In addition to mirroring your sketch, you could skip the step of converting the mirrored half to ref lines and just do a 180 deg revolve.

 

[JohnRBaker]

Perhaps, BUT if you DO create your 'Diameter' expression as a 'User Defined' expression, that will automatically make it available to you from within the Part Navigator under the item titled 'User Expressions', which means that you can go there and edit the value for 'Diameter' directly without even having to know that there was a sketch or where it is or anything.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[fighterpilot]

John,

I understand the power of expressions. However, I could just modify the diameter dimension in my drawing and edit it there as well or just double click the feature and edit it there.

Where is the class "UGNX5 for the Former Pro/E User"? I need that class. It may clear up a lot of questions I have. Today I'm busy adding dimensions to features in a drawing. I already put the info into the feature/sketches. In Pro/E, I'd just "show" them. I'd also be able to use the drawing to back drive my model. I'm not finding how to do that in UG either. I know at one time you mentioned I could show my dims in UG but I'm not finding how to do that.

Now I'm just complaining....

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

If your models were created with sketches and you use any of our Drawing templates, or create your own, sketch and hole feature dimensions will automatically be added to the drawing views. If you don't use drawing templates, but just create your drawings using the menus and dialogs under drafting, then after your views are placed, go to Insert -> Feature Parameters... When the dialog comes up, it will indicate which features are available for having their dimensions created automatically from their definition and you select the items you wish to inherit dimensions from, select the view you wish to see the dimensions in (note that for sketches the view has to be at least parallel to the original sketch plane and for holes, you have to actually be able to see the hole feature in the view selected). As for editing the dimensions of a sketch from the drawing, that is ONLY supported if the drawing is in the same part file as the model and then that's done via accessing the expression editor from within the drafting task.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[acciardi]

John/Fighterpilot:

The advantage Pro has when 'showing' feature dimensions in a drawing is that you can click right on the part feature in the drawing view and preview the dimensions intrinsic to that feature and select only those you are interested in.

With NX, you are shown a table with all the model parameters in it, and you have to somehow know ahead of time which parameter is associated with which feature. My models have thousands of dimensions, so it's not a very practical way of showing dimensions. This isn't a training issue, it just is one area where I'd like to see NX show more graphical ineraction.

 

[MCGNX]

"This isn't a training issue, it just is one area where I'd like to see NX show more graphical ineraction. "


Here, here, and I'm not a pro/e user either but this is still something I would like to see work better. (not the diameter dimensioning, but the showing of editable feature params on drawings)

 

[JohnRBaker]

It's interesting to note that when we first introduced this ability to edit the parameters of a feature from within a drawing, albeit by accessing the expression editor, our two largest customers at the time (and one of them still is and the other is in the top 10) demanded that we TURN THAT FEATURE OFF IMMEDIATELY because, as they put it, under no conditions will they allow people who create drawings to edit the models that these drawing were being created from. That's not their responsibility and it must be prevented by the software. So we had to add an environment variable (they wanted something that the average user couldn't find and then change) that would disable this 'feature' while in the drafting module.

After we got that reaction, we decided that perhaps it would be a waste to expend any future resources enhancing this if our largest customers had already told us that it would never be 'appreciated' by any of their users (and perhaps even their suppliers if they had their way). Now we've never taken a survey, but I suspect that there may be other customers who have similar attitudes and have availed themselves of this 'option' as the variable is fully documented in the 'ugii_env.dat' file.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[cowski]

fighterpilot,
Concerning your sketch question, you got some replies the last time in thread561-213151. I agree that a diameter dimension in a sketch should be an easy thing. This thread and the previous one give some decent work arounds for now.

 

[hudson888]

I have used the mirrored method in sketches in the past. Although John's expression based method is probably more sound. The good thing that you may not know about those expressions is that they can be effectively built in by editing the sketch dimensions during the process of creating your sketch. You can rename the parameter number of each dimension to something easier to find in the expression editor later on, and you could simply perform the multiplication or division calculation inside the dimension value.

And I can also report that it isn't just NX that doesn't automatically support an extra function to perform the simple trick of division and multiplication by 2 that it takes to recognise a diameter and a radius or vice versa. I think you'll find the each different CAD system deals with it differently.

I suspect that the reason that such a class is diffiuclt to find is that the former Pro-E users would probably expect an NX user to teach the class and therein lies a difficulty in finding such a person prepared to put up with constant cries "Why doesn't NX do it just like Pro-E?"

I think that new to NX users need to accept that there are two perfectly good ways to achieve this simple result and enjoy the experience of using either or both.

Cheers

Hudson