Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Milling a half round groove and using a slitting saw

Anonymous

Milling a half round groove and using a slitting saw

Anonymous
Not applicable

Hi Guys,

 

I could use some CAM help. I have a project where I am cutting a 1/16" wide slot down the length of a 5/16" aluminum rod. I designed a fixture with a half round groove on top and a matching clamp block. I want to use a 1/4" ball mill to cut the groove. I tried every CAM option I could to mill the half round groove but Fusion wwouldn't let me select the face of the groove to mill.

 

The second issue I had was cutting the slot in the rod. I'm using a 2.75" x .063" slitting saw. The slot doesn't run the entire length of the rod, only about 80% so I designed it with a 2.75" radius at the ends so the saw could ramp into the slot.

 

Can any of you get this to work?

 

Thanks!

 

 

Chris

1 Like
Reply
Accepted solutions (1)
3,284 Views
18 Replies
Replies (18)

jeff.walters
Advisor
Advisor

sounds like you just want to use a 2D contour for this. insted of selecting faces try selecting edges. 

Jeff Walters
Senior Support Engineer, CAM
0 Likes

Anonymous
Not applicable

Jeff,

 

I tried that and it just selects one of the flat rectangles at the top of the block.

 

If you have time please open the DB and try it yourself.

 

Thanks,

 

 

Chris

0 Likes

Anonymous
Not applicable

Hi Chris,

 

Go back to your model and add a workplane tangent to the bottom of the groove, or use an offset workplane.  Draw a line on that workplane to act as a path you want a tool to follow.  Return to Cam and use the Trace toolpath (I couldn't get this to worlk with Engraving so use Trace).  Select the line you drew when in the the Geometry tab.  In the Passes Tab, checkbox Axial Offset Passes to control your depth of cut/# of passes.  See the attached images and I hope it helps.

 

Mark

1 Like

Anonymous
Not applicable
Thanks Mark. That gets me closer. I'm not dogging your solution but I could do that in SheetCAM. I wanted to use a 1/4" ball mill to cut my 5/16" groove though. I thought that was within the power of these fancy 3D CAM tools. :^)
0 Likes

Anonymous
Not applicable

It usually is whithin the power of the fancy CAD/CAM tools but it can be frustrating at times.  But I hear ya!

 

I had trouble doing this on your part so I drew a new model and extruded a circle to make the cut you're looking for.  It worked on my model so maybe look back at your modeling methods so see if something is affecting that surface you want to machine.

 

See the attached image (of my remodel) with a Parallel toolpath found under the 3D dropdown menu.  My model has a sketch that acts as a bounding box for containing the tool.  Your stepover amounts may need to be made smaller because the .250" ball mill takes up a lot of room in your grove diameter of .312.  Again, I hope it helps ya.

 

Mark

 

 

1 Like

Anonymous
Not applicable

Interesting. So maybe the fact that I cut more than 1/2 of the circle away caused Fusion to not recognise the feature. I'll try that tonight

0 Likes

Steinwerks
Mentor
Mentor

First thing to EVER do in CAM: add your Model to the Setup.

 

Model Setup.JPG

 

Next, you have to define the part of your part that you wish to machine. I've attached your part with a new setup. I modified your original 2D Contour to be a little nicer on the tool, added a contour to cut the ends, and a Parallel toolpath to cut your slot. There are a good number of parameters to play with but this will work. You'll have to figure out what the best stepover/stepdowns are, and the correct feeds and speeds for the material and your machine obviously.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
1 Like

Anonymous
Not applicable

I think that was the problem. I selected the model then selected a 3d parallel path and it seems to be working now. I've only been doing 2D ops on single body models so far so maybe that was why I hadn't run into this problem before.

0 Likes

Steinwerks
Mentor
Mentor
Accepted solution
If my post was your solution, it'd be great if you could mark it as such.
Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

Anonymous
Not applicable

Chris,

 

I remodel your bottom jaw and I didn't have to select the model in the setup section.  I still got the parallel toolpath to work.  Edit: But since your model is a quazi assembly, I think Cam doesn't know which body you want to machine so you have to select the model in the setup section.

 

I attached my model if you care to look it over but it's just one model and missing the top clamp.  Therefore, I didn't need to select in the setup section.

 

Mark

0 Likes

Steinwerks
Mentor
Mentor

@Anonymous wrote:

Chris,

 

I remodel your bottom jaw and I didn't have to select the model in the setup section.  I still got the parallel toolpath to work.  However, with your model you do have select it for the setup so the toolpath generates.  Not sure what's causing the difference in your model vs. mine but I was able to get it working without using the model in the setup section.

 

I attached my model if you care to look it over.

 

Mark


I'm sorry, but this isn't making the feature he wants, and that can be seen in the Simulation:

 

Parallel.JPG

 

Without selecting any sort of geometry the software is just making a sort of approximation based on your bounding area.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

Anonymous
Not applicable

You have to extent the bounding box for containing the tool.  I just made it arbitray hoping he would catch onto the  idea of using a containment.  Also adjust the bottom height plane to keep it from making that dive after leaving the part.  I didn't even mess with feeds and speeds, just trying to get a path to generate.

 

Mark 

0 Likes

Steinwerks
Mentor
Mentor

@Anonymous wrote:

You have to extent the bounding box for containing the tool.  I just made it arbitray hoping he would catch onto the  idea of using a containment.  Also adjust the bottom height plane to keep it from making that dive after leaving the part.  I didn't even mess with feeds and speeds, just trying to get a path to generate.

 

Mark 


The reason it wouldn't generate properly in the OP's file is that he had not chosen a model or any geometry. I suspected that adding another body into yours would break the toolpath, and I was right:

 

Broken Parallel.JPG

 

Without specifying the model in the Setup, the toolpath defaults to whatever model is sitting in your boundary sketch. The only thing I did to this file was create a shaft in the pocket as a new body, hid it (lightbulb) and regenerated the Parallel operation.

 

If one ever wants to program in assemblies (and it really works well in Fusion), the model has to be selected. After that, selecting fixtures can help with collision detection and other issues.

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

Anonymous
Not applicable

I really like your toolpath, I would only hog out with a striaght pass before running that program.  Just to lighten the load on the mill.

 

How did you select the containment boundary without drawing a bounding box?  When I select the surface it works but not as good as your containment.

 

Thanks,

Mark

0 Likes

Steinwerks
Mentor
Mentor

I've created a Screencast that I'll attach to this post when it's done uploading. Essentially you just select the boundary of the feature as you would for a 2D Contour operation.

 

Here's the link: https://knowledge.autodesk.com/community/screencast/adfa6b46-0950-40db-ae1e-e73239d349f0

 

Hopefully it's done processing by the time someone reads this Smiley Wink

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
0 Likes

Anonymous
Not applicable

Thanks for the screencast and I saw how you selected to boundary conditions.  That cleared up a few things for me and it worked.  But I also tried the checkbox under model and selected the surface to machine.  That worked as well.

 

One additional way is to use the Avoid/Touch surfaces and checkbox the Touch surfaces at the bottom, then select the surface to be machined.  So it looks like there are 3 good ways to contain the tool and I'll no longer draw a bounding box.  That was just coming from an older CAD/CAM technique and being applied here.  Time to throw away those old tricks.

 

Thanks again for your help.

 

Mark

0 Likes

Steinwerks
Mentor
Mentor

I will simply add that the default consideration in Fusion 360's CAM is that you select the model in the setup. This applies (3D) toolpaths in a model-aware fashion. I will say that until my current job (and we don't use Fusion) I was also used to the old way: mostly 2D paths programmed in whatever CAM package I had, previous jobs including Mastercam X6 and GibbsCAM 2012+ for which models were used sparsely if at all.

This is not that CAM. :winking_face:

Neal Stein

New to Fusion 360 CAM? Click here for an introduction to 2D Milling, here for 2D Turning.

Find me on:
Instagram and YouTube
1 Like

Anonymous
Not applicable

OK Adam,

 

I selected the model and used Mark's idea of drawing a line to do the roughing pass and then a rectangle as a boundary to contain the operation. Then I watched your screen cast and figured out that you are using the <Alt> key to select individual edges to create the chain that you want to machine. I hadn't seen that trick before. I guess I really need to go back and watch all of the training videos. 

 

I have the 3d operation on the 1/2 round working now. Now I need to see if I can get the slot cut on the rod. I may just sketch the path I want the tool to follow.

 

Thanks to both of you for your help.

 

 

Chris

0 Likes