Moving from Wildfire to NX4

Hello all - I'm a longtime Pro/E user who will be transitioning to NX4 due to my company being bought by a larger outfit. I have NX4 installed and running, and I'm looking for some insights on how to best start part/assy models.


In Pro/E, datum planes are the starting point of every model. As the model progresses, it is good practice to always reference the three primary datums while placing features. NX doesn't seem to require this - you can sketch on the WCS plans.


In general, can someone please summarize what is considered best practice for build models in NX?


Also, I notice that sketches do not seem to get sucked into the model. The sketch outline is always visible.


Any pointers to best practices or tutorials appreciated. Note - I have not had formal training yet, but I want to get a jump on things.


Thanks and best regards.


Ed Acciardi, Seagate corp

welcome to nx. while nx does not require the basic datums it is good practice to create themand use them like you did in proE. when you insert a sketch you'll see a previewof a sketch datum and horizontal reference axis. just ignore these and select oneof the datums you created explicitly instead. once you select your sketch placement datum the "preview" datums will go away and a temporary wcs will appear. x is horizontal, y is vertical and the sketch will be oriented with the z-axis pointing at the user. nx assumes the horizontal reference based on your current view so there is no need to select a horizontal reference axis or plane unless you want it to move relative to something. here's the process in a nutshell: create the 3 fixed datum planes. orient your view to the view that you want to sketch in. select insert>sketch and select the datum plane you want to sketch on. click the green check or MB2. you can also create a sketch by first selecting a datum plane and then right clicking and selecting sketch. this avoids the confusion of those pesky"preview" datums.

Thanks - I appreciate the prompt response.


Is there any way to get the sketches to absorb into the model? Can they be put onto a layer and blanked?


I have to say that with my few hours with NX, it seems very powerful and flexible. It seems like there are many options for everything. Pro forces you to do things its way. For example, in Pro, you can only revolve a section around a sketch centerline. NX lets you revolve around any line or edge anywhere in the model. Pretty cool.


Ed Acciardi

Ed, the sketch is treated as a feature in UG, this allows you to sketch several profiles at once and use it over and over again. I set up my sketches to be on a layer and then toggle the layer on and off.


Steve Calvert

Hi Steve - yes, I've noticed that you can select individual curves within a sketch to use. This lets you use a mega sketch for many different operations.


As I mentioned elsewhere, I am pretty impressed with how flexible NX is. I can use it almost exactly like Pro/E if I want to.


Ed

Hello. As far as making sketches invisible try to select the sketch on the feature tree and right-click it. I don't remember it exactly, but it should give you the option to make it internal to the extrusion. I will check it at work and tell you the exact way.

You can create sketches as part of the extrusion feature in NX4. This way the sketch "hides" once you create the extruded solid. If you need to edit the sketch simply edit the extrusion and the sketch is there. If you want to see the sketch you can select Show/Hide from the model navigator. It is amazing how much the CAD systems are getting more and more alike. Catia, Pro/e and NX now all have similar functions.

I like nx!

i want to know more about the nx4. i had learned the 18.0.but i am little used in practice.so i am not very farmiliar about it. who cansupply some good tutorial and practice for me.thanks firlst.

Hello Friends ,<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />


I am a novice in UG, But I had the samedoubt asMr Acciardi & after some work I found to bring fixed datum always in the beginning , All you have to do is go to pull down menu INSERT/ DATUM POINT/DATUM PLANE (sub menu) then you have to pick the WCS which will be in the middle of screen. This will generate three fixed planes.









Edited by: josho3630

There is a Datum CSYS feature which will create an Origin Point, X Y
& Z axes and XY YZ ZX Datum planes all in one feature. If you like
having Axes and Planes on different Layers you can do that as
well.



I haven't used NX4 yet but have one question about the sketch internal to the feature.

Can a sketch made before the Extrusion be converted to an internal
sketch as you can do on Wildfire. In Pro/E there is a break link option
which will copy an existing sketch and make it part of the feature and
leave the original sketch intact.



The one nice thing that I loved about NX is that you can transfer
between the show and no/show spaces easily . I have the comand Ctrl+Shift+B
Reverse Blank All programmed on my space ball. You can even
do part operations and switch between them during feature
creation. In Pro/E when a layer is hidden there is no way
to view it in the no/show space.



Another good shortcut key is Ctrl+Shift+U which will unblank all items that are hidden without having to go to blank space and then blank all the hidden options.



Michael