newbie (from Pro/E)

[jdkl]

I come from the Pro/E world,
and now in the near future I will have to use NX.
No training is planned, so I'll have a go at it on my own.
Starting with this :

http://etm.erciyes.edu.tr/dosyalar/dokumanlar/Shaper Tool Head Assembly.pdf

So, now my question :
Would there be helpful people around there that might help me during my struggle with this ?
Answering my stupid questions each time I can't figure out how it is done in NX ?

For example :
I have designed the back plate as a revolved body.
Now I want to create the dovetails by removing the unwanted material. I sketched the cross-section of the cut I want to make,
but now some questions arise :
- the sketch is overdimensioned, and I seem to be unable to delete dimensions : how is that done ?
- using Pro/E wording, I now want to make a cut, both sides, through all (starting from the sketch plane, remove all material defined by extruding - to infinity - the sketch in both directions) : again : how is that done ?

Thanks to anyone who takes the time to answer these (and I hope : future) questions.

Jan (from Belgium)

 

[joycejo]

You should start with the help docs there are a lot of good examples of using the multitude of features in NX.

Do you have CAST?
As you review some of the posts here you will find several links other other training sites and links.

Back to your original question. When in the sketch you can delete dimensions using the delete function or selecting the dimension and pressing delete. You may need to turn off the auto dimensioning option.

When you extrude the sketch you can choose the boolean operation for the extruded solid (tool body) in this case select subtract.

You do not need to extrude it to infinity but only to the next face or selected face. This will keep the distance of the extrude associative to the target body.



John Joyce
N.C. Programming Supervisor
Barnes Aerospace, Windsor CT
NX6.0.5.3

 

[jdkl]

Thanks John, that was quick !

Pressing delete did nothing, now it does. My fault, I guess.

And the cut also is straightforward, once you get used to the NX wording. start and end "through all" did it.

Now I copied and pasted a sketch, I can change all dimensions, but how do I change the sketching plane ?

 

[jdkl]

Unfortunately, when I change the dimensions in the copied sketch, the original is also changed. Is there a way to "unlink" them ?

 

[jerry1423]

As far as asking questions goes . . . you are able to do a search in here that will probably answer many questions that you have.
Don't hesitate to use information from versions of NX earlier that what you are using because many times (but not always) it will apply to the version that you are on.

 

[Toost]

When you paste the copied sketch, there are three expression options, "create new, link to original and reuse original"
If you select the "reuse original" both the original and the copy will use the same expression, and there are no way ( known to me) to make the copy independent.
The option "link to original" creates linked expressions ( such as p22=p12) which is simple to change/ break. ( the first sketch will drive the copy)

 

[jdkl]

Hi Toost,

You are very helpful.
I did not realize "reuse" was irreversible.

By just starting with a not altogether simple example,
and aiming at what is possible in Pro/E,
I guess I will master NX to an acceptable degree in a matter of days.
The exercise at

http://etm.erciyes.edu.tr/dosyalar/dokumanlar/Shaper Tool Head Assembly.pdf

has about everything straightforward mechanical design requires.

If I can get it done, with the help of knowledgable people like you and John, I will be "up and running" in a fraction of the time a regular training would take.

The details and fancy optimisations can then be learned while I am already doing useful work ...

 

[jdkl]

Everything was quite straightforward ...
(see screenprint - bad display quality : using NX in a VM)
Now I try to make drawings.
Getting a drawing view is easy, but the assembly shows up rotated.
(the assembly is tilted in the view).
What must I do to have the assembly correctly oriented in the view ?
In Pro/E I would make the coordinate system of the first component coincident with the coordinate system of the assembly, or I would align the datum planes that are based on the coordinate system, but I do not find this possibility in NX ?

 

[DaSalo]

When you create your drafting view there is an orient tool on the view dialogue window that will allow you to specify your view orientation relative to geometry in the assembly. There is a check box to toggle whether the orientation is associative or not.

You can also define a custom view. I usually do this while still in modeling. Orient your WCS so that the Z- axis is along your view direction and the X axis is along the view horizontal.

View=>Operations=>Orient --- This will snap your view to your WCS orientation.
View=>Operations=>Save As --- This will save the current view under a new name.

Make sure you don't bump the Spaceball or otherwise move the view between the Orient and Save As operations.

Now when you go to create a view in drafting your new custom view will appear in the drop down list along with all of the standard views.

I usually create a few custom views to capture the orientations that I will need most frequently and then use the View Orient tool if I find I need a few more orientations as I go along.

If I suspect the model will be revised in a way that could affect the drafting views I only use the View Orient tool as this is the only way that I know of that will create an orientation that is fully associative to the model geometry.

Hope that helps.

NX 7.5.4, NX 8.0.1.5
Tecnomatix Quality 8.0.1.3
PC-DMIS 2011 MR1