This area seems like it should be no problem to fillet, but it fails at any radius larger than .002".. Any ideas on how to get this to work?:
Here is the curve:
Here it is happy with the setting of r=.002":
It's hard to diagnose the problem without playing around with the actual file. Could you attach it? In general I'd try different options like face fillet and play around with the various settings.
upload your file
I've got a simplified version of the part ready to share, but I can't figure out how to attach it... Do I need to use a 3rd party server?
Devin, We have the same problem here where I work all the time. We are forced to do top down design work and are stuck with customer geometry that is normally suspect. Every day we are forced to try to find the problem area that Solidworks does not like. One of the things I do is to go to the tools drop down and click on the :"check". Use stringent
check box, and keep your fingers crossed something pops up that you can address. What you are looking for is a area on the model that has some sort of miss match, or an edge that isn't quite right. In my opinion the fillet tool in Solidworks is the only part of the software that could use some work. Over the many years of running and trying every trick in the book there are always those models that just fight you all the way. Good luck, I hope this might help you.
Devin, as Bill said, it's hard to diagnose geometry problems without the file, but if I ran into this problem, I'd take a series of diagnostic steps to discover the cause and location of the fillet failure.
For the failure of what appears to be a straight-forward fillet, I would follow Bill's advice and check for geometry errors using the "Check" tool he explained.
Bad geometry can be produced by the source application (esp. if it's not a Solid modeler), the SolidWorks import engine, lofts, boundaries, shells, fillets and just about any other feature. SolidWorks will sometimes give these errors a pass if you have 'verification on rebuild' turned off.' You can find that control in the Options dialog under System Options: Performance. If that's unchecked, check it and then rebuild your part (CTRL+Q) and see if any of your other features produce errors.
Try those remedies and let us know what happens.
OK, here is the file:
I was able to get it to work using the Asymmetric option in the fillet parameters. This may be new to 2015.
Hope this helps,
Dang! Yeah that doesn't exist in 2014! Shoot.
There is most likely another way to get it to work, possibly others will reply with an alternate solution.
here it is with a bigger fillet
had to take the extrude down blind past the surface
Hmmm that is interesting! Funny thing is it won't let me do .015" radius which is what I wanted. .02" did work though! Some progress!
When you change your fillet to 0.015" does it still work? Errors for me.
Thanks in advance,
Nope. Error at 0.015". Builds at 0.020" or the 0.030" you had saved it at.
wont work at .015
doesn't like the radius on bottom
I think the reason that SW will not do the fillet is because of the curvature of the fillet around the bottom, if turn on curvature under the evaluate tab you will see by the sharp contrast in the colors that you do not have a nicely blended fillet around the inner edge of your part. I think this is why SW will not filet your part
this is with zebra lines turned on
I changed the lines and arcs in your profile sketches to splines using the fit spline command. Now I am able to use various sizes of fillet. Have a look at the attached file
Paul, thanks for the tip! Interesting as all the sketch relations were tangent and I thought everything would be OK.. But yes, changing to fit splines did make the model fillet without hassel!
If you can modify the Inside Bottom2 sketch rad from 0.010 to 0.012,
the fillet 0.015 will work
Hope this works
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