Solidworks surfacing accuracy

I have created some surfaces using various lofts and fills and tangency controls at the edge connections to each other. I can even stitch the surfaces together.
Yet, when I take section cuts through the surfaces I am getting mismatches of 0.00004" between curves. At what accuracy does Solidworks ignore these mismatches and can the NC guys ignore them at this level of mismatch?
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Phil,
That's pretty good. I don't think the CNC is going to track that small a difference. Look at Ed Eaton's presentations on surfacing. What you are seeing occurs when analytical and non-analytical surfaces match up. It would be a bigger problem if you were meshing the model for FEA.
I'm curious whether TOOLS/CHECK also spots the mismatch.
I have seen surfaces go off more than that along guidelines. What is more, this can change from release to release on the same model.
When I was modeling some really small parts with .001" radii this kind of thing was a problem from time to time.
When it comes down to it, SW is a digital representation of a real part. There are going to be tolerances and mismatches due to the digital nature of the computer.
TOP
On Aug 21, 11:46 am, Phil Evans ( snipped-for-privacy@tagaerospace.com) wrote:

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Tools/Check is picking up surface edge gaps of 1.9685e-007 in
I am surprised Solidworks has this accuracy built into it.
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How did you come by the .00004" number then. In CAM?
TOP
On Aug 21, 12:32 pm, Phil Evans ( snipped-for-privacy@tagaerospace.com) wrote:

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I took section cuts through the surfaces and measured the mismatch of the none continuous curves that occured at the surface boundary.
I don't know why the values are different.
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Do the parts made from the files pass the test of form fit and function?
Bob
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The NC guys have told me thay can produce within plus minus 0.005" which is way tighter than I need. Aerodynamic surfacing is usually acceptable within a surface profile geometric tolerance tolerance of .030"
I guess I was wondering if a step of 0.00004" would cause the NC guys a problem and secondly at what tolerance does Solidworks ignore mismatches. It has obviously ignored this mismatch in the surface stitch function but not in the section cuts.
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The problem I see continually is that some (all) of the CNC software that is out there will "see" these minute gaps and refuse to generate a toolpath. It then is possible to increase the surface tolerance number and the collection of surfaces can then be machined. The downside to this is that the finish of the cut is then deteriorated proportionally to the amount of tolerance increase. On many parts, this isn't a problem but on say a mold, the finish (as machined) won't be acceptable. If there aren't any "gaps", is is possible to create almost a mirror like surface finish. Of course, this comes at the expense of increased machining time.
I am going through this right now with a SW created model. There doesn't seem to be a simple solution and if there is one, I would certainly like to hear about it. I have heard talk of "healing" software that would allow a person to work with and correct these types of problems.
This "problem" is certainly not unique to SW. I see the same geometry from other CAD programs. There is always some translation involved in bringing non-native geometry into a CAM program but, IMO, the source of the "problem" lies with the creation software for model (or surfaces group).
Gary
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Well I guess if the NC guys relax the surfaces by 0.00004" the mismatch will disappear. This will certainly not affect the finished surface functionalty from my perspective.
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Every case seems to be different. If you can live with the resulting surface finish after the "adjustment" then you won't have any problems with this approach.
Gary
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A lot of this is dependent upon the parasolid modelling kernel. Once one ventures beyond conics and planes, surfaces and their intersections and edges are calculated as an approximation and an allowable error.
UG (back in my UG days) gave direct control over the parasolid tolerance, allowing one to tighten or loosen on a feature-by-feature basis. SW does not.
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Catia v4 also allowed the setting of the allowable mismatch before the system considered entities to be a single entity. By default it was 0.0004"
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CATIA translations I worked on had a much higher allowance for out-of- square entities to be considered parallel or perpendicular. This was a pain when bringing CATIA sheet metal into SW, where faces in the source CATIA model were off enough that SW considered them not parallel.
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Phil,
    Solidworks has always been a bit sloppy on accuracy. Especially on surface continuity, that is fundamentally why it works however, the surfaces don't converge mathematically as tightly as you might think. C2 continuity was not introduced until SW2007. On the other hand that is also why complex fillets, etc.. fail. I don't know the magic number to the first question. Perhaps SW can chime in on that. But my guess is you are right at the SW limit.
To answer the second question. Better NC systems allow you to set the tolerance, to whatever you want it to be. 0.00004 is not a problem for me. Even if it gets to 0.0004 it is not a problem, I can compensate. The better NC systems, show you the gaps. A majority of the time it is not a big deal, but sometimes it is. Either way, we deal with all the time.
clay a_design
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Phil,
    Solidworks has always been a bit sloppy on accuracy. Especially on surface continuity, that is fundamentally why it works however, the surfaces don't converge mathematically as tightly as you might think. C2 continuity was not introduced until SW2007. On the other hand that is also why complex fillets, etc.. fail. I don't know the magic number to the first question. Perhaps SW can chime in on that. But my guess is you are right at the SW limit.
To answer the second question. Better NC systems allow you to set the tolerance, to whatever you want it to be. 0.00004 is not a problem for me. Even if it gets to 0.0004 it is not a problem, I can compensate. The better NC systems, show you the gaps. A majority of the time it is not a big deal, but sometimes it is. Either way, we deal with all the time.
clay a_design
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