NX6 Modeling - how to dynamic section/clip a pie wedge?? 1

[GoHokiesGo08]

Forgive me if this has been posted before, I tried searching a few terms without any luck.

I'm working in NX6 in modeling and trying to generate a clip/section view of my model for presentations. We work with a lot of cylindrical pressure vessels at my job, and for presentations we prefer to show the models with a pie wedge/quarter quadrant removed from view, ie - leaving 3 quadrants of the cylinder still visible, with only one quarter quadrant removed, like a piece of pie removed.

Every time I do this now, I have to save a separate assembly, link all the bodies, then trim it into quarters to blank one quarter of it from view.

There must be an easier way!! The Box option creates the opposite of what I want by allowing me to clip the three quadrants instead of removing just the quarter. And parallel planes, obviously, wont let me create perpendicular cut planes.

Any ideas on how to do this using the clip work section feature?

Thanks!!

 

[JohnRBaker]

OK, there are two approaches that may work for you.

The first is to use Assembly Cut, which will modify ONLY the assembly file (the component parts will remain unmodified so all you need to duplicate is the assembly file). With this you open your assembly, create a solid body representing the 'space' you wish to remove and then use...

Insert -> Combine Bodies -> Assembly Cut...

...where you select as the 'target' (the components you wish to be modified) and the 'tool', the body representing the 'space' to be removed'. The result is an assembly where the modified parts ONLY exist in THAT particular assembly. Also this is a feature which can be toggled ON/OFF by simply suppressing the 'Assembly Cut' feature.

Shown below is an image of what his looks like (I've left the 'tool' solid visible so that you can see how it was done:

Note that you can edit this 'feature' so that you can add or remove components from the cutting operation until you get the exact result you desire.

The second approach, 'Section View' (don't confuse this with drafting sections, as this is done in the model), is much slicker in that all it does is create an edited view where the rest of the assembly model views remain unchanged, however it works in a similar manner except that you don't have to create a 'tool' solid ahead of time as that step is built into the function itself. Again you pick the components to be modified and then a 2D profile (which could be a sketch so that you can edit the 'tool' profile as well) representing the cross-section of the swept volume of 'space' to be removed from the model. To use this function go to...

PMI -> Section View...

This is what this looks like below (note that this picture was taken during the creation of the PMI Section and shows the 'tool' being swept but before the operation was completed. When completed, the result would have been the same as seen in the Assembly Cut image):

Now there is one caveat: while the 'Assembly Cut' functionality is part of basic NX modling, 'Section View' requires the purchase of the PMI module. Now this module IS included with many of the NX bundles so you may already have access to it.

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.

 

[GoHokiesGo08]

John - you're a genius, my friend!

The PMI Section View is exactly what I was looking for and lets me make a quick sketch to get my pie wedge removed. Excellent! I like how I can save multiple views as well in any shape.

We just upgraded from NX3 to NX6 a few weeks ago (took my company forever to upgrade), so I haven't seen the PMI functions before. Looks like there some pretty cool stuff you can do with it. I'll have to teach a few of the guys here the new trick I learned from you.

Thanks again, exactly what I was looking for.