Pro/E user attempting switch to UGNX 6

[fighterpilot]

After over 10 years as a designer and CAD admin for Pro/Engineer I need to learn UGNX 4. This is proving to be quite difficult. I'm sure I'll have more questions but I'll start with this one. I have a cylinder 10" in diameter, 8" long and want to create a turned down section 4" in diameter and 5" down the axis.

I want to revolve a rectangular section about the axis of the cylinder to create in Pro/E terms, a revolved cut. I can seem to get the rectangular section created in UG sketcher but now I'd like to apply a diameter dimension in my sketch (4") to what would be the OD of the revolved cut. In Pro/E sketcher I would just drop a centerline down the center of the part, align it to the existing cylinder axis then dimension the revolved cut by selecting the sketch line, centerline, and then the sketch line again. Viola, I have a diameter dimension. How do I accomplish a similar scheme in UG?

Next I would like to constrain the other section line to the projected edge of the main cylinder OD and then constrain the bottom edge of the sketch to the lower edge of the large cylinder. In the end I want two dimensions driving this cut, the 4" diameter and the 5" cut length.

How do I go about doing this in UG?

Thanks...

--
Fighter Pilot
Manufacturing Engineer

 

[NXMold]

" In Pro/E sketcher I would just drop a centerline down the center of the part, align it to the existing cylinder axis then dimension the revolved cut by selecting the sketch line, centerline, and then the sketch line again. Viola, I have a diameter dimension. How do I accomplish a similar scheme in UG?"

You dont. Diameters, for the most part, simply do not exist in UG. You can't specify them, you cant measure them, its a mess. If you need to, you can dimension the radius from the center to the edge, and type 4.000/2 as the dimension. Unlike proe any expressions you enter will be retained (where proe solves the expression and stores the value only).

You might want to try drawing two concentric circles on the same plane, 10" and 4" diameters. Extrude the large one 8" long. Extrude the small one with a start value of 5, end 10, a two-sided offset of 0, 3, and a boolean subract. Just another way of looking at it.

I switched jobs about four months ago after using Proe 2001 for 8 years, now I use NX5.0.2 and am loving it. Interpart modeling is in the stone ages compared to proe, but direct modeling and all the flexibility are great. I hardly use any sketches anymore, I find the UG sketcher quite cumbersome though its hard to pin down why.

 

[JohnRBaker]

I assume that you don't want to create the original cylinder with a sketch since that would have made this exercise so simple that it wouldn't be worth the electrons to respond.

Therefore I create a 10" dia x 8" long cylinder as a primitive and created the 'Turned-Down' section with a subtracted revolved feature using an embedded sketch. To make it easy to edit the size of the 'Turned-Down' section, just open the file attached below and go to the Part Navigator, expand the 'User Expressions' item and now you can edit the "two dimensions" of the 'Turned-Down' section.


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/

 

[acciardi]

You've hit on several limitations of sketching in NX. The inability to dimension a revolved diameter has been covered, but it is also not possible to directly access silhouette curves that do not lie within the sketch plane.

You'll have to create isocline curves before the sketch feature, or, in the case of a simple cylinder, you can 'project' the face edges of the cylinder and make some reference entities using the quadrant points, and then align to the reference entities.

 

[JohnRBaker]

I suggest that you look at my model for a much more direct means of solving the so-called 'silhouette curve' problem.

As for the 'diameter' dimension issue, anyone who thinks that it's hard work to use the expression system to create a diameter expression that is used to drive the sketch dimension via a math relationship is just looking for stuff to complain about.


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/

 

[phillpd]

John,

The issue with having to use "Radius=Diameter/2" is that you can't edit the diameter without going into the expression editor.

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[PhilJenkins]

I just wanted to say that I made the switch from Pro/E to NX several years ago and, although some things are initially more difficult, on the whole NX is a far easier system to use, it is more flexible and more enjoyable. You will soon learn to disregard the Pro/E way of working and learn how NX does things. I still use Pro/E where the client requires it but my default system is NX without question.

 

[hudson888]

I think you're all missing the point that just because there isn't something in NX that is analogous to the way it is done in another CAD system that you have been used to, doesn't mean that the method you first thought of is the only one or even the best way to create that particular geometry.

You could use a primitive with bosses and grooves to define a turned part just as easily as you might sketch it.

Or you could just create a sketch with mirrored elements about the centerline that allow you to dimension across the diameter. I achieved the whole model in one feature for what it is worth.

Best Regards

Hudson

 

[fighterpilot]

I looked at the way JohnRBaker and hudson888 did their model construction and understand both methods.

When I constructed models in Pro/E the mindset I had when creating them is "will I need to turn this feature off" So keeping in that way of thinking I constructed them in ways I knew would allow that. Hence my reason for not creating my revolved section like hudson888 did. There is no way for me to turn off the turned down section. Now the way JohnRBaker contstructed the model probably lends itself to supressing the turned down section if I needed to. I'll eventually figure out how to do that in UG.

Now, let me talk about the dimensions specifically. Again, I constructed models with dimensions I knew I was going to tolerance in the model and then SHOW in the drawing. I have seen many "glassy eyes" around here when I mention "why can't I just show my model dimensions?" So when I dimension a diameter in my sketech and tolerance it in my model I know thats what I will see in the drawing. If I want to flex my model dimensions in an assy tolerance stackup which was available in the assy mode of Pro/E I can do so by just flexing the diameter dimension.

Lastly, if my drawing represents what I actually modeled in the drawing I don't need to worry about someone coming along and detailing my drawing and possibly dimensionsing a feature from other surfaces that might not represent what I intended in my model. This is what really floored me about UG. You create your model and then you have to create a drawing by adding new dimensions. Well I my former world, the dimensions and design intent was already in the model.

Maybe NXMold and JohnRBaker could give some comments about my topics above. I'm not opposed to learning UG, I just need to understand some of the whys.

Thanks...



--
Fighter Pilot
Manufacturing Engineer

 

[NXMold]

I never used that dimensioning ability in proe, I always created new dimensions on drawings. Now in NX I hardly create any drawings at all. However, I understand what your driving at because I always created geometry and dimensions in a way that reflected intent as much as possible, such as if I was modeling something from a print I would try to use primarily the print dimensions while modeling (avoiding entering a radius in the model where the print specifies a diameter). That kind of 'interpetation' may seem very basic and easy to people limited to working that way, but having seen and used the alternative I know that it does lead to problems regularly.

Another note, you've probably already found that you cannot create centerlines or mirrored constraints in sketcher, but the system can when you mirror geometry. That one blows me away. So you could take Johns model, mirror the inside edge of the rectangle, make it a reference line, and add your diameter dimension. Thats probably impractical for the most part though.

 

[acciardi]

fighterpilot:

One more comment...

I've been using NX for two years now after 14 years with Pro/E and I have *maybe* reached 50% of the productivity I had.

My job involves making essentially the same parts over and over again with many small changes, so a parametric approach has proven to be the fastest. We do not use any primitives or direct modeling with NX - we start and end every model with 100% sketch-based design.

You *can* use NX in about the same way that you used Pro, but you will spend more time in your sketches. We stubbornly insist on 100% trimming and constraining every sketch even though the system does not require it. We do it because we feel that it conveys design intent better than untrimmed sketches.

My point is that if you try to use NX as an exact Pro/E replacement, you will experience some frustration. You have to decide whether to use all the modeling techniques NX offers and make your life easier, or stick with what you know and force the system to be used in a way that it can handle, but not as smoothly as Pro did.

There are tools in NX to accomplish whatever you want, but you'll have to depart from the Pro/E scripted way of doing things.

 

[cowski]

acciardi,

Pardon my ignorance, but what do you mean by "trimming" sketches?

 

[fighterpilot]

cowski,

I believe acciardi means close off your sketches. Good sketch practice, as I was taught, always closed sketches. We aligned to existing edges when we needed to and essentially always told the system "cut out this specific area or make this specific extrusion"



--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

phillpd,

If you look at my example part attached to my original post, you will note that you can edit both parameters of the 'turned-down section' from the Part Navigator, without ever having to open either the sketch task or the expression system.


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/

 

[JohnRBaker]

cowski,

The reference to not trimming a sketch might refer to the technique which we call 'select intent' where irrespective of whether the sketch curves were fully trimmed or not, the user is able to explicitly define which sections of the sketch profile, including defining what I guess you call 'virtual' trims on-the-fly, when using a sketch when creating a solid or sheet body feature. This allows several things including not having to waste as much time in the sketching getting every single curve trimmed-up so that there is only one single unambiguous 'loop', which often takes most of the time. Also it allows for the creation of filleted corners while still constraining them to the theoretical sharp corners of the an un-filleted profile without having to either trim the curve to the fillets and thus needed to add additional reference curves that need to then be constrained and dimensioned.

Note that this 'selection intent' approach is something that was adopted from Ideas that had something called 'hay-stacking' which did the same thing. Once you know how it works, you can save yourself a lot of what some people call drudge work when putting those last touches on a complex sketch.


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/

 

[MCGNX]

Dont' know if it's been mentioned, but you can get a diameter dim by mirroring your sketch and then dimensioning to the OD. You can then either convert the second half to reference, or simply revolve your sketch 180 degrees

 

[acciardi]

MCGNX:

Yeah, I'm kind of anal about the whole design intent thing, so that's exactly what I do - mirror the whole sketch about the revolve axis.

Ed

 

[hudson888]

I just wanted you to duplicate it and manipulate the dimensions so that you can see that they work off the mirrored half allowing it to work on the diameters. I think that's pretty clever.

Cheers

Hudson

 

[phillpd]

John,

I guess you're referring to User Expressions ?

And if a user expression wasn't used ?

Specialty Engineered Automation (SEA)

http://www.sea4ug.com

a UGS Foundation Partner

 

[JohnRBaker]

The whole purpose of it being limited to 'User Expressions' is so that the list is not just another 'print-out' of everything that's in the Expression System. Granted, this might require the user to create a few redundent expressions such as:

Diameter=10
p2=Diameter

'Diameter' shows up in the list of User Expressions while 'p2' does not. This way the user can control which parameters are exposed the world and which are not.


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/