By curved surfaces, if you mean you're doing 3D surfacing, watch your scallop height. I use about .0005 if I don't need a smooth surface, and anywhere from .0001-.00005 if I want a smooth surface. Of course, the lower you go, the more CNC code you get...
Can u send <?:namespace prefix = st1 ns = "urn:schemas-microsoft-comffice:smarttags" /><st1:City w:st="on"><st1lace w:st="on">ur</st1lace></st1:City> part file so I will check the problem and give u a machine file
<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" /> [email protected]
Accuracy determines the length of the smallest edge Pro will recognize in your model, or the largest gap between 2 edges that will still be considered joined. Relative accuracy is ratio between the smallest edge in your model and the longest dimension across your model. Absolute accuracy is a specific dimension for the smallest permissible edge (or the largest permissible gap) in a model.
If a part is 20" long with relative accuracy of .001, the smallest edge Pro will recognize without geometry check errors is .02". If the same part has absolute accuracy of .001, the smallest edge recognized is .001".
The tolerance parameter in the machining module is the width of a deviation band that a cutter can travel before another line of code is generated to correct for a change in direction (it controls the length of the cutter path polyline segment)
Eddie's explanations are right on. I would like to also add to it what this means as far as machining.
From a manufacturing point of view, a relative accuracy setting means absolutely nothing. You must find out what is the equivalent absolute accuracy setting in order to ensure that your tessilation problemis not coming fromit. This will ensure that your edge descriptions are within your machining capabilities, and therefore your surface quality high enough. Additionally, as a rule, always make sure that your manufacturing assembly (the same goes for mold assembly) is set to absolute accuracy, and that the absolute accuracy of the assembly is equal to the equivalent absolute accuracy of the part (regardless whether the parta accuracy is in absolute of relative).
In your NC sequence parameters, set the TOLERANCE parameter to 1/2 your machine fraction capabilities (usually 0.001 in mm and 0.0001 in inch). This is most important if youare machining surfaces with low curvature. It will generate more point (larger NCL file and longer compute time), but will keep the tool closer to the true surface definiton.
To check on the problem, do the easy thing first and just crank up the TOLRERANCE value. If that still does not work, you have to fix the accuracy. I recommendsetting absolute accuracy to 0.001 in mm and 0.0001 in inch if you need your surface very smooth.