1. Parasolid with tolerant modelling up to 0.00001; this is the largest tolerance we usually use if necessary. This will depend on the original model.
2. Acis o.oooooo1
3. Step o.oooooo1
4. Iges o.oooooo1
The above three have the almost same tolerance for import. This tolerance may be loosened to 2.5e-5 meters according to the original data for import. For export, it’s the same as #1 (1.0e-5 meters).
SolidWorks uses the following tolerances on the surface trimming curves when exporting as IGES (trimmed surfaces):
High trim curve accuracy: 3.0e-6 meters
Normal trim curve accuracy: 1.0e-4 meters
When exporting as “STANDARD” we do not apply a surface tolerance. When using the STANDARD setting the surfaces are exported as analytic representations where possible and as B-spline surfaces for those surfaces which do not match an analytic form. The tolerance of these surfaces will be whatever tolerance they are represented as natively in SolidWorks – for analytics this is 1.0e-08 meters.
When exporting in anything other than STANDARD setting SolidWorks will export all surfaces as B-splines. Existing B-spline surfaces in the model (e.g. lofts, sweeps) will be exported to whatever tolerance they are currently represented with in SolidWorks (typically ~1.0e-06 meters). When converting analytic surfaces (i.e. planar, cylindrical, spherical etc) to B-splines for IGES export we use the following factor for the B-spline approximation:
0.5 * trimmed_curve_tolerance
There is no way to manually adjust the tolerance of imported data. SolidWorks will automatically apply tolerances based on the accuracy of the data. SolidWorks default precision is 1.0e-08 meters, but any data accurate to between 1.0e-06 meters and 1.0e-08 meters should import successfully.
I have never worried about the accuracy of my exported files, assuming that it would be better than the molder could cut the mold. (Thanks, Alin, for the Knowledge Base numbers that confirm that!) I worry more about whether or not all of the geometry is in the file, so that the person importing doesn't have to guess what my design intent was. I assume that Parasolid is the best for export, being the native file for SolidWorks, if the importing software can handle it. STEP seems to be the second best, with IGES in third place. In theory, ACIS should work well if that is the native file format for the importing software, but it always seems to take much longer than the others and is much more likely to crash SolidWorks on large files.
The best method is to send multiple file types until you work out with the importing users which one works best for each. It is also a good idea to round trip the exported files to see if they are good when you import them into SolidWorks. That doesn't prove that they are good going into the importer's software, but it is liable to catch some errors. I am too lazy to do this on all files, usually only checking when someone complains that my exported file has problems on their system.
I think it answers my question. I have similar system of sending multiple standards and it was the difference in their size what made me question tolerance. (.x_t is noticeably smaller then .STEP, etc)