Trouble milling corner relief with ballnose endmill

[ARMTooling]

I had posted a few months ago asking for help with a ballnose endmill tool path and tried using the method suggested with varies options changed to suite this particular cut but I'm still not getting the results I'm looking for. I've attached a file showing what I've done so far, the current state of the tool path doesn't remove enough material and I can not figure out what I'm doing wrong. I don't know if it is in my work planes being used to orient the tool or if it's in the tool path parameters. Any help would be greatly appreciated!

Thank You

[dylan_smith]

Hi @ARMTooling,

Could you export your file as a .f3d please, this file type doesn't consolidate the data inside of your project, it separates it all into different files.

Thanks,

[ARMTooling]

Sure, but I don't see an option for f3d file export, am I missing something?

[seth.madore]

File > Export > Save to local folder. If the file contains linked components, they should be broken first before exporting..

Alternatively, you can right click on the file in the Data Panel and select "Share Public Link" and make sure the file is set to "Allow Downloading of items". Paste that link here.

[ARMTooling]

Thank you Seth, I had to break the links before the option of .f3d would be available.

[dylan_smith]

@ARMTooling  could you be more specific by showing me which areas you want to remove the material?

Thanks,

[ARMTooling]

I hope I attached the screenshot correctly. This is the operation I'm having trouble with...

I would like to clear out this corner with a ballnose end mill and I've been trying to use the Parallel function but I haven't had much luck as you can see.

My plan was to enter in towards the center of the pocket (left) and mill outwards (right), stepping down if need be for stock removal.

The corner is modeled .125" wide and full radius so I was trying to use a 1/8" ballnose end mill.

[ARMTooling]

for added clarity, here is another look with the areas shaded

[dylan_smith]

@ARMTooling the radius of the area selected is around 3.2mm and your tool is 3.175mm, there isn't enough room for the tool to operate, so I'd suggest using a smaller tool. Also parallel probably isnt the best tool path to use, I'd personally use steep or shallow if you have the extension, if not, scallop.

Thanks,

[ARMTooling]

Thank you Dylan,

I do not have steep and shallow, I want to say I tried scallop but I will give it another shot, I'm still very new to Fusion 360 and it's been years since I've done CAM.

Also, you said the tool is too big for the feature as it is and to use a smaller tool, would this be your suggestion for scallop as well?

[dylan_smith]

@ARMTooling Yes definitely. Any toolpath you decide to use needs a smaller tool than you're currently using. If you use a smaller tool you will see much better results than you're currently getting.

Thanks,

[ARMTooling]

I've tried a smaller diameter ball nose endmill without any better result. I've also tried the scallop operation and I still can not get the tool to get into the deeper (right) side of the relief. Any thoughts?

[dylan_smith]

Hi @ARMTooling,

Looking at the plane you've used for the 3+2 movement and the gap you have for entry, you will need to cater the tool size for this size gap. Also, the accessibility analysis picture shows how much of the radius you can get from the angle you're using. 

You will need to play around with the angle you come in at, and also make sure your tool is small enough to get through the gap. I don't believe you will be able to cut the radius in one go, it will be a case of using a lot of different angles to remove as much material as possible.

Fortunately you won't have to do this for every instance, you will be able to pattern your toolpaths 5 times around the centre of the model.

I hope this helps.

Thanks,

[ARMTooling]

Dylan,

I believe I get the part about the accessibility analysis, basically I need to tweak the angle of the orientation plane to until I get the entire relief corner in green?

As for the gap, I'm not following there. If the tool enters towards the middle of the pocket it would never be near that gap as I'm not machining that area or accessing what I'm machine through that area. Could you explain that a bit more?

Thank you again. Sorry for all the questions, I have everything else on this part figured out but this feature, this is only my second part I've worked on within Fusion 360.

[DarthBane55 · Accepted solution]

Sorry to barge in this, but I saw the picture and got interested.  I would do it with Trace operation, as per picture below.

I also posted your file back with my operation in it.  I had to draw a sketch to drive the toolpath, you can unhide it to see what I did.  I hope it helps.  I simulated it with comparison mode and it all showed green.

Note: I didn't check the direction of X-Y axis, so you'd have to tweak that, and I also didn't play with S&F at all, basically I just made a toolpath but didn't tweak anything.

 

[ARMTooling]

Thank you DarthBane55! That's more of what I had in mind. Looks like that will work, thank again!