Hi folks
I'm trying to create a fillet for the following profile (for machining purpose) but not able to do so. Kindly help me in finding a solution or work around to create a fillet.
Thanks
Unable to create a fillet
Did you create the model in Fusion? If you did can you share the f3d file?
Mark Hughes
Owner, Hughes Tooling
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I've experimented with this a bit and there are 2 problems.
First problem is the curves in the DXF are not tangent between each curve and there are also some short lines that cause problems after adding the draft. In the attached file I added tangent constraint (note this did change the shape. You need to do this yourself and get the best fit to the original).
After cleaning up the curves and extruding the biggest fillet I could get was 3.3mm. The limiting factor is this face in the hook area. When the fillet gets too big this surface is totally consumed and Fusion fails to fillet.
As an experiment I split the part and filleting the rest of the profile seems OK.
Here I moved the hook area to another component. Hook area 3.3mm radius, rest of model 4mm.
I've attached the model, it might help you figure this out. One thought is you might be able to use a variable fillet and just reduce the radius in the hook area.
Mark
Mark Hughes
Owner, Hughes Tooling
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Here's the best I can come up with using a variable fillet. In the selected area the fillet starts a 4mm then reduces to 3.3mm.
@jeff_strater I noticed a bug in the Variable fillet, when you try and edit the feature it shows an error because the start and end positions are changed. Start becomes -1.0 and end 2.0. They should be 0.0 and 1.0! File's attached.
Mark Hughes
Owner, Hughes Tooling
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@MetalRipper_ wrote:
This part was modelled in solidworks. f3d file is not available
Well you'll need to recreate in Fusion because the STP file has the same problem as the DXF where there's very bad tangency between curves.
You'll need to insert the DXF and delete the outer offsets so you're only left with the inner shape. Then clean the profile up adding tangent constraints and remove any short segments without changing the shape too much.
Mark
Mark Hughes
Owner, Hughes Tooling
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@MetalRipper_ wrote:
This part was modelled in solidworks.
Whoever modeled this in SolidWorks does not know how to use SolidWorks.
The sketch is at the Origin in one corner - but not constrained to the Origin. This should be automatic.
Many of the dimensions are unnecessarily duplicated.
When I start to add some of the missing dimensions I observe that they do not make logical sense...
Missing all Vertical, Horizontal and Tangent relations (except on some holes).
This should be all automatic.
The entire story hasn't been revealed?
(Was this imported into SolidWorks from AutoCAD?)
The deeper I did into the geometry the more issues I find.
Based on my observations I would not trust the geometry and in fact would make a wager that it doesn't represent the true Design Intent.
All of the effort to create Fillet feature is useless if the base geometry is flawed.
I see this issue across users of all CAD softwares.
