Projecting a Solid Body onto a plane as a sheet 1

[jmiklovic]

Does anyone know of a way to project a solid body onto a plane and have the output be a sheet body or an outer profile curve.

The goal here is to take a converter housing casting and get a projected area without the aid of mold wizard.

Currently I have been extracting all the edge curves of the casting and projecting them to a datum plane, then trimming up the outer profile to get a closed section and taking the area that way.

I attached a picture if that helps.

Jay Miklovic
Sr. Design Engineer
Edco Inc.

 

[JohnRBaker]

What version of NX are you running?

Starting with NX 8.5 we added an option to the 'Extract Curve' function of NX that will make this a fairly straight forward effort despite the fact that it will take a couple of steps to accomplish, but in the end, compared to your current approach, it should be much quicker.

First thing you need to do is make sure that there's a datum plane, either a separate feature or one of the three planes of the CSYS, which when viewed parallel to the screen, that the desired profile of your model is also parallel to the screen. Note that at this time, if you normally work with the 'Perspective' view option toggled ON (which I always do), please toggle it OFF so that you're working in a parallel view. Now it's critical, at least during the first part of this workflow, that the datum plane that you want the outline of your model to be created on remains parallel to the screen so don't accidentally rotate the view. Also, this will only work with Solid models.

OK, now that we've got your Datum Plane parallel to the screen and your model situated how you want it and in a parallel view (i.e. not a perspective view), and at the this point, you might want to change your Work Layer so as to help manage the display of the resulting curves later on. So if we're ready, go to...

Insert -> Curves from Bodies ('Derived Curve' in NX 9.0 and NX 10.0) -> Extract...

...and select the 'Precise Outline' option but do NOT select the OK button. Rather simply hit Cancel since the curves will have already been created.

OK, from here on you don't need to worry about not rotating your image. You may want to now set a new Work Layer and turn off the layer where the model is located as long as you can still get access to the Datum Plane that you want your final profile on. Now go to...

Insert -> Curve from Curves ('Derived Curve' in NX 9.0 and NX 10.0) -> Project...

...and select the curves that you just created and project them onto the Datum Plane (make sure the 'Along Face Normal' option is used). BTW, at this point, since the original 'Precise Outline' curves are not associative you might as well turn OFF 'Associative' when performing the 'Project' option so that you can get rid of all of the extra curves without messing-up anything.

So now you have only the 2D profile of you model and nothing else. Note that this will also work with Assemblies, even if the Components were loaded using Lightweight Representations.

Anyway, I hope this helps.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[jmiklovic]

Absolutely beautiful. I am in NX9. Worked perfectly. This just saved us a whole bunch of time.

Jay Miklovic
Sr. Design Engineer
Edco Inc.

 

[wkellen]

This is very helpful! We have been looking for an easy way to do this for a long time. Now, is there a way to do this where it will be associative? We have to enter projected area of a part, a feed runner, and a vacuum runner into a spread sheet for PQ^2 along with volumes of each. We always drop the ball when something changes and the spread sheets will be wrong. We are looking to put this on a print so the values are constantly updated. It gets labor intensive when the parts and runners are not flat to a plane. If the "precise outline" could be made associative, the rest is easy.

Thanks,
Wayne