[BarnBurner]

I use Rhino 3D to make solids, and made some parts with pockets that exported as .dxf and worked perfectly in MasterCAM.

Next I tried to use the Rhino 3D Fillet command and then generate G-Code with MasterCAM, and I could not get it to recoqnize the Fillet. I tried it many different ways, but no luck.

Anyone know how to do that?

I am using MasterCAM 7.2 Mill, and the newest Rhino.

[cadcam]

Did you check Normals ?

[BarnBurner]

I could only find Test norms, and Check model under

Analyze: Surfaces:

That didn't work, it just kept telling me to Try Again

The part I made is a 3D Solid, not surfaced. It was extruded as a solid, then 'difference' and 'Solid fillet'

I don't know exactly what you need to know, so tell me what info would explain this better.

[cadcam]

So you are using version 7.2 with solids am I correct?
and you are trying tool path the solid or the surface from a solid?

Can you eamil me you file

[BarnBurner]

>So you are using version 7.2 with solids am I correct?

Yes

>and you are trying tool path the solid or the surface from a solid?

I want it to add a fillet to the top oustide edge of a pocket; the part was extruded as a solid.

>Can you eamil me you file

I could send you the .dxf.

[BarnBurner]

ACAD 2000 .dxf exported from Rhino

[cadcam]

BarnBurner, may I have the Rhino file as in MC V9.1 you are able to bring direct Rhino files in.

thanks.

[BarnBurner]

The .dxf is exported from Rhino as an Acad 2000 .dxf.

I have added the .3dm.

Not sure how that would help me anyway, as I am only running 7.2.

[cadcam]

ok the problem is there is no surface to surface with.
What type path do you want to use?

I can make a surface on it to make it work and give you back an Iges to bring in to 7.2 mc and cut it.

[BarnBurner]

That would help me with this, but could you possibly tell me how to do it myself using Rhino or within MasterCam?

I'd like to be able to do it myself, and have tried for days; there is just something I'm missing...

[cadcam]

Ok now I need to know are you going to surface the path or use a radi tool being a 2d path?

[BarnBurner]

I wanted to surface it so it could be cut on the X and Y axis', and stepped on the Z.

The mill I have is screws, not ball, so if it steps alot on the Z, it leaves ridges.

[cadcam]

Here is an iges of your file that has the surface mad from a arc and the profile using the Create, surface , sweep option.
then we can work on tool paths.

[cadcam]

Just so you know DXF does not support Surfaces. But as I can not makeing true solids .
Rhino is a surface base software not a Solids base software.

[BarnBurner]

Your file worked perfect, but I was unable to duplicate it.

Can you tell me what program you used for the cut/sweep? And possibly explain abit how you editted the file I sent you?

[BarnBurner]

Can anyone else here help me with this problem? I would sure appreciate it!

[HuFlungDung]

I'm just looking at your 3dm model in OneCNC. Its only a 2d wireframe from what I can see, but by looking at the rounded end of the pocket you are trying to fillet, I see a potential problem: the underlying geometry is faulty in the sense that the straight edges are not tangent to the end arc (near the red lines). This is the case both on the outside profile and the inside profile of the pocket. This kind of geometric problem creates a difficult area where the semi-circular fillet meets the straight edges. If the geometry really has to be that way, you'd likely have to make seperate solids and cut them (with solid cutter operations) to fit at such a joint, but you could not fillet across such a joint with a surface fillet function. Just IMO

Both rounded ends of your model display the same mathematical inaccuracy. Start over from the basic wireframe profile, delete the lines joining the arcs, and use some kind of tangent line function to redraw the lines truly tangent to the arcs. Retrim the arcs and try again.

What looks okay in some softwares is not acceptable in others, mainly due to tolerance settings. Obviously, Rhino did create some kind of surface fillet, but it wouldn't be strictly legal as one surface. There would have to be another fillet where the arcs meet the non-tangent lines, to create a true tangency. Then, you might have a sound surface fillet that will export correctly.

[cadcam]

Well to do what I did I used Mastercam.
As for brining in your file ther were no surface contained in the DXF file as DXF does not support surface data.

But in MC 7.2 you can use the option of

Create
Surface
Swept

this will prompt for how many across default "1" enter then pick one of the .625 Radi you have.
then the along will be the top profile that conects to this radi around the part.

As for waht kung Fu said about the radi and the other line not being tangent is true but you still can create this surface and cut it is is just funky as they are not tangent as they should be.

I had my my self fixied this on the file.Cant remember if it was on the one I sent you.
Sorry about the long delay as I have been real busy.

I have on at least one of my box Mastercam V6.1,V7.2,V8.11,V9.1 & MC Beta X so i can followup on past versions of MC.

Will rhino let you out put a Iges or SAT type file.
If so this will support Surface data.
Would Like a Iges file from it if possibale.


As for making a single surface with the none tangency you will need to set Sync to Entity to support the sharp intersection.