rotate an imported model for good part compare (part file)

Hello,
I have a model that was send over as step-file to the toolmaker. I got
it back (as step-file) with a few modifications. Now I would like to
make a volume compare between the original and the modified. Then I saw
that the modified didn't had the same orientation. The original had his
bas on the bottom plane while the imported step model had it on the
front plane. A compare is useless.
What can I do? I do not know how to rotate the imported feature
(step-file) in the part file. Or can I say on wich base plane the
imported feature should come?
Johnny
Reply to
johnny geling
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You could redefine the view orientation
say the original part view is top set the view orientation/elevation so you have same view as on the original part hit the spacebar to bring up orientation dialog, click once on top, in dialog list to highlight, then click Update standard view button in the dialog (2nd from right), Both views should match !
Neville Williams Z-Axis Design - NZ "remove the KNOT to reply"
Reply to
Neville Williams
Try assembling the two parts in an assembly maybe? I don't know if there is a way of doing a boolean op to get the volume difference tho'...
Just checked - there is no option in SW to import a file (STP, IGS) to a pre-defined CSYS :-(
Reply to
wurz
But there is a copy/rotate feature. I used that. Then the volume compare fails. Is that a good tool?
Johnny
Reply to
johnny geling
Is the imported part a watertight solid? Are there any free edges?
Reply to
wurz
If you get it into the right orientation with the copy/rotate feature - try to export it again to loose the parametricity - maybe that helps.
Reply to
Ivan
Hello Johnny-
1. You can add your own Reference Geometry System to any SolidWorks part. This controls the orientation of the X,Y,and Z axis. With an imported part: a. Open the .step file and create a new SW part file. b. Orient the Part correctly. c. Insert, Reference Geometry, Coordinate System. Again, chose the correct orientation of the three axis. d. Now, export the part as a .step file, chose Options, and chose the new Coordinate System. e. Open this new .step file and it will be orientated correctly. f. See the Help file for further information.
2. To compare two part documents, use SolidWorks Utilities.
Best Regards, Devon T. Sowell
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Reply to
Devon T. Sowell
Why don't you just do an insert-part (base part for us older guys). Use the body move/copy tools to get it in the right location and then just use a combine-subtract feature?
Sometimes this is easier for me to see correct orientation than the solidworks utilities for comparing geometry.
--Matt Feider
johnny gel> Hello,
Reply to
Matt Feider
Hi Johnny -
Two things to try.
1) Compare assembly wtih parts laid on top of each other by mating - easiest method in my mind. mentiond already
2) Open up the step file, define a coordinate system based on the "other" models origin and re-export, then pull back-into an assembly over the top of the original. (Export) Output does allow one to define the origin at the time of output, so when it is reimported, it will come in on top of the the other model. A lot more work than above, but something to bear in mind as possibly useful, particularly for those in CNC programming who need to define a given coordinate system upon import (happens some times).
I've used method 1 a thousand times to validate a change to an original or "my" model to "their" model. Is even a great method for modeling when you need to hijack "their" geometry (particularly used when making a poorly behaved dumb solid into a full parametric model when featureworks is underpowered - about 25 percent of the time). When I worked as a fabricator, I used this one quite alot - more that I care to remember. If I had a nickel for evey time I used it I would have 100 bucks . . . um . . . wait . . . I do have a hundred bucks . . .
Later,
SMA
Reply to
Sean-Michael Adams

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