Data loss while exporting 1

[sluzzer]

What is the best practice & format to control data loss while exporting the model?

I created a midsurface for an aerofoil blade using 'mid-surface' option. It looked fine (i mean, exactly at the middle) in the NX, but when i import the model in another CAM software, I found the midsurface was slightly skewed. I exported using IGES format with model tolerance 5 microns.
What is the reason for this change and how to avoid this?
I am using NX9

Thanks.

 

[niedzviedz]

Try different export format. I think that for some software the best is parasolid, for others step. IGES has one biggest disadvantage - it only generate sheet bodies.

With best regards
Michael

 

[Toost]

Two questions,
why sending a midsurface to a cam -system ?
2) does it look skewed of is it skewed ?

The graphics , what you see on the screen, is not the same as the actual surface.
CAD systems which use NURBS data will based on the Nurbs data tesselate the surfaces, and what's shown on the screen is the approximated -tessellated version. These display-facets might sometimes fool the user into believing he has a poor model / better model than what it actually is.
This is also the reason why you sometimes need to do "Update display" in NX, the display facets are too large / crude.

Regards,
Tomas

 

[sluzzer]

Toost,
1. It is required for Spiral finishing operation in CAM. The tool path and orientation are calculated based on the Midsurface.

2. It is actually skewed. I get a error message of 'Midsurface touching the side faces' in CAM software.

 

[Toost]

1) try other file formats, such as Step and Parasolid or JT. The IGES file format has not been updated since 1996.
2) the only reason i could guess is that the CAM system isn't using NURBS math for surfaces /solids. ( Most CAD systems uses NURBS.)
Or that this CAM system has some form of limitation in how it can handle NURBS data.
I have seen an example of this many-many years ago, The solid in NX "exploded" in the CAM system. - the blend faces was far away from the surfaces it should be tangent to.
IN that case, the CAM system had a limitation on surfaces to not have a polynomial exponent higher than 3, and the NX blends , when exported became 4 or 5.
the CAM system then recreated ( new) surfaces, but which wasn't identical neither in shape nor position.

in NX you can see the exponent and the number of patches by Information - Object and then select the "face" ( not the feature but the face of that midsurface)
"Degree in u and Degree in v
then "Number of patches in u and v
If the degree-s are higher than 3, you can try Extract Geometry- face and select the option "Polynomial cubic", this will then create a 3x3 degree surface which you can try exporting.


Regards,
Tomas