The big question- new to NX7 but Pro/E user for 15+ years. 2

[pete3000]

OK.. no where on the web have the small community of "pro/engineer migrated to UG" people put info for newbies moving from Pro/E Wildfire 4 to Unigraphics.

In Pro/E we are used to seeing auto-dimensions and constraints pop up in sketcher. all of which are weak until you confirm them as strong or leave them as is. In pro/e the sketches are always constrained when you exit the sketch. Can NX7 auto-dimension as you sketch? if so, how do we turn it on? I saw the Auto constraints function.

How to i make construction geometery in the sketcher in NX? In pro/e we can draw a circle or line and flip it to a construction entity. future extrusions etc, ignore the construction entities.

I have never seen so many numbers go flying across the screen as I do in NX7. In Pro/E the only numbers we ever see are the dimensions we modify. I am constantly seeing X Y and Z boxes everywhere.

I have lots of good things to learn as a veteran pro/e user of surfacing, cabling, routed systems designer, etc...

I look forward to a long discussion..

 

[JohnRBaker]

Auto Dimensioning of Sketch curves are supported in NX 7.5, which work very similar to the way you've described what you're familiar with.

As for what you call 'construction' curves, in NX these are known as 'Reference' curves. Any curve (or dimension) can be converted to being 'reference' by selecting the curve (or dimension) and pressing MB3 (Mouse Button 3) and selecting the 'Convert to Reference' option from the pop-up menu.

BTW, while many people feel that Sketches should always be fully-constrained, in NX there is NO requirement that they be before they can be used to create a feature such as an Extrude or Revolve.

As far as the X,Y,Z data entry widgets (X,Y when working in s Sketch) are concerned, in NX whenever you're selecting points on the screen, particularly when creating curves, these provide you the option to immediately enter explicit 3D (2D in a Sketch) parameters of the points without having to enter a secondary dialog or trigger some alternative parametric scheme. They also serve the purpose of reporting the current 3D (2d in a Sketch) location of the cursor as you're creating curves.

Anyway, if you have any other questions, please post them and well try to fill in the 'gaps'.

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.

 

[pete3000]

Thanks John. Would it be possible to request an enhancement for a User Role that would say "ex-Parametric" user or other types of CAD software?

 

[looslib]

We needed the reverse of that where I used to work as they switched from UG after 15 years to Pro/E because of a corporate decision. The division got sold a few years later and the designers had to switch again to CATIA.
The ones that had been there the whole time had great resumes: 15 years UG, 7 years Pro/E, 4 years CATIA.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[fighterpilot]

pete3000,

Good luck making the switch, I'm still struggling still almost 3 years later. Taking some of the formal UG training classes helped but it's a real struggle moving from the way Pro/E modeled things to how UG wants them. I'll disagree w/ JohnRBaker on the constraining of sketches, I always constrain mine to remove ambiguity, and, I always use sketches. Big thing when I came over was why were people using tool solids with subtractions, unions, etc. I never remembered using those in Pro/E. I still don't use them in UG. Another thing that bothered me in UG. When doing a revolved section you cannot dimension a revolved diameter in the sketch, only the radius. Seems like UG likes to work in radii rather than diameters. Not really sure why. Oh some will say just write a relation or make a parameter, but why? Just let me dimension my diameter in the sketch.

I find UG drawing cumbersome as well. Assembly mode seems bothersome too. I could go on and on about things that don't make sense to me but I won't.

The reality of it all is I doubt I'll ever be as efficient in UG as I was in Pro/E.

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

My comment about using less than fully-constrained sketches was just to make the point. With NX you are NOT required to have a fully-constrained sketch before you can move to the next step. I was not advocating that it's a good idea to leave your sketches in an ambiguous state, just that it was up to the user to decide whether or not to do so, rather than the software.

As for your comment about NX tending to only work in 'radius mode', it's just a matter of how you approach the problem. Since in NX the sketch is in reality a separate feature from the solid (although if used as intended, the user may not notice this) when creating the sketch the system does not know how it's going to be used so it does not recognize that one time a dimension is linear and the other it's going to represent a radius/diameter. So in this 'linear' world, a length has the same meaning as does a 'radius' since they are only measuring the actual distance between two points, whereas a 'diametrial' dimension implies something quite different. However that being said, if you really wish to create your sketches for rotated parts in such a way that you can directly enter values which represent diameters rather than radii, thus avoiding having to create expression relationships, you can do what I do when that is what I really want, as seen in the simple example that I've attached.

The key thing to remember about NX is that there are always 10 ways to do anything. Unfortunately, 9 of them are perfectly valid. Therefore it's up to YOU to decide which is the best approach for what YOU are doing AT THAT MOMENT.

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.

 

[fighterpilot]

John,

We haven't moved over to NX7 yet. Can you redo that example in NX6?

--
Fighter Pilot
Manufacturing Engineer

 

[JohnRBaker]

OK, here's basically that same model, except it was created in NX 6.0.

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.

 

[pete3000]

in sketcher how do I apply a symmetic constrain on 2 end points across a centerline. I see a MIRROR constraint being applied when i mirror an object, but how do i do this with say, creating a rectangle across a centerline?

thanks in advance.

 

[JohnRBaker]

Can you provide at least a picture of what you're trying to sketch?

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.

 

[pete3000]

simply draw a vertical line. turn it to reference. now create a rectangle starting to the right of the line and bring it across the centerline. the centerline should divide it perfectly. In pro/e symmetry contraints pop up when you reach the proper distance on the left side of the centerline. I expected the mirror contraints to do the same thing but they do not. This is a very, very common technique used everyday within pro/e.

 

[JohnRBaker]

There is no Symmetry constraint in NX 6.0 but there is in NX 7.5.

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.

 

[pete3000]

John, would there happen to be some documents/presentation describing the new functions of 7.5 vs. 7 on the Siemens website? I refer to it before asking anymore Qs. thanks!

 

[looslib]

There should be a What's New guide.

whatsnew752.pdf
whatsnew751.pdf
whatsnew75.pdf

These do require a webkey to access!


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

In this and other recent threads, there have been requests for how someone could go about receiving training in the latest capabilities of NX and while there is always the opportunity to take formal training at a Siemens office or from some other provider of training classes and material, there is also the opportunity to participate in FREE online 'webinars' covering various topics related to the use of many of the software products from Siemens PLM Software. If you might be interested, below is a link to the current list of webinars planned for this coming March:

http://training.industrysoftware.automation.siemens.com/promotions/announce.shtml#webniars

Also note that near the bottom of the page there are a couple of links to the replays of recent past webinars.

Note that if you sign-up for any of these events you'll have an opportunity to be put on a mailing list so that you will know about future webinars far enough in advance that you can fit them into your schedules.

Anyway, this might be something which may be of interest to some of you.

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.