Trying to surface machine with a radius cutter

[Kyle F]

Hello everyone, I'm having some trouble with a project I'm currently working on.

I'll attach some screenshots to further explain my issue, but long story short I have a full radius saw blade in an arbor + hardholder. I just drew wireframe on a separate level and linked that geometry to create my custom tool. 

I have a full multi-axis license but this job will be on one of our 3 axis mills. Essentially I roughed the part with a shellmill and now I need to address the undercut sections, where I plan on roughing + finishing with this full radius saw cutter (aluminum).

Ideally I'd like to rough this area with an opti-rest but I just can't get the toolpath to mill the undercut section. I also have tried a few different surface finish toolpaths for the finish passes but all to no avail,.. this leads me to believe maybe my issue is in my tool definition, should I maybe try to create the tool as a slot mill instead of custom tool? 

the geometry of the undercut is pretty simple so I'm not too worried about the opti-rest failure because I could always just have a few seperate contours of various depths/multi-passes to rough, but I would really mainly like to get the surface finish figured out because programming that "manually/old school way" is definitely possible but certainly a pain in the butt lol.

I appreciate any feedback or help!

[crazy^millman]

Define as a slot tool not a custom. Unified will work in 3 Axis machines. Just change to 3 Axis in Tool Axis Control. I am not sure who Opti-Rest would handle this. I might do 2D HST in sections and go about it that way. Draw each tangential intersection of the tool to the surface at each depth of cut. Then work out the profile from each of them. Remember the Unified supports stock models and has Morph Pocket in the Roughing.

[Kyle F]

On 9/1/2023 at 7:30 PM, crazy^millman said:

Define as a slot tool not a custom. Unified will work in 3 Axis machines. Just change to 3 Axis in Tool Axis Control. I am not sure who Opti-Rest would handle this. I might do 2D HST in sections and go about it that way. Draw each tangential intersection of the tool to the surface at each depth of cut. Then work out the profile from each of them. Remember the Unified supports stock models and has Morph Pocket in the Roughing.

Thank you so much, I'll give that a try. 

and by the way ron, I really appreciate you and all the interview/video content you've helped to create on youtube. It has helped me a ton! I've been a lurker on the forum for a while lol

[crazy^millman]

48 minutes ago, Kyle F said:

Thank you so much, I'll give that a try. 

and by the way ron, I really appreciate you and all the interview/video content you've helped to create on youtube. It has helped me a ton! I've been a lurker on the forum for a while lol

Well thank you for saying what little i have done has been a help.

[JoshC]

for how simple that shape is you can even use this path shown here to get it done, assuming you fix the custom tool like mentioned above and re-define it as a slot mill https://blog.caminstructor.com/cutting-3d-forms-with-2d-toolpaths

[Kyle F]

52 minutes ago, JoshC said:

for how simple that shape is you can even use this path shown here to get it done, assuming you fix the custom tool like mentioned above and re-define it as a slot mill https://blog.caminstructor.com/cutting-3d-forms-with-2d-toolpaths

I'll give this a shot for the finish pass and see how that goes. thanks for your input.

[danatoem]

not sure what i am missing on this but I often did this kind of shape with flowline ( have to uncheck gouge check!) and had good results.  See screen shot.

[Kyle F]

1 hour ago, danatoem said:

not sure what i am missing on this but I often did this kind of shape with flowline ( have to uncheck gouge check!) and had good results.  See screen shot.

I have found the issue!

so I tried flowline like you posted and it still wasn't quite working out,.. which led me to try and re-create my slot tool (again lol)

this time I didn't link to any custom level geometry, so it's essentially the same except when I don't have the arbor cap drawn, it cuts correctly.

quite odd but something with that geometry hanging off the bottom of the radius cutter, masetercam doesn't like it for my toolpath.

I'll just extra careful when proving out the program in the simulator to ensure the cap won't collide with anything, this shape is simple enough it shouldn't be an issue.

 

[JoshC]

11 minutes ago, Kyle F said:

I have found the issue!

so I tried flowline like you posted and it still wasn't quite working out,.. which led me to try and re-create my slot tool (again lol)

this time I didn't link to any custom level geometry, so it's essentially the same except when I don't have the arbor cap drawn, it cuts correctly.

quite odd but something with that geometry hanging off the bottom of the radius cutter, masetercam doesn't like it for my toolpath.

I'll just extra careful when proving out the program in the simulator to ensure the cap won't collide with anything, this shape is simple enough it shouldn't be an issue.

 

its because your driving to a Square or sharp corner tool on the left side, your rendered mastercam tool and rendered imported tool need to match properly, so you need to start with a Slot mill tool not a custom tool, here is a video i found after a quick search that shows how we need the parametric values to match the imported tool 

 

[danatoem]

also flowline allows you to extend the cut motion off the part by using the "gap-settings" - "Tangential line length" !

[Colin Gilchrist]

Also, you can use "Direction" button to give you "surface lead in/out" motion, to get the tool in/out of the cut. For undercutting operations, you want to disable all of the "gouge checking" options.

[Kyle F]

26 minutes ago, JoshC said:

its because your driving to a Square or sharp corner tool on the left side, your rendered mastercam tool and rendered imported tool need to match properly, so you need to start with a Slot mill tool not a custom tool, here is a video i found after a quick search that shows how we need the parametric values to match the imported tool 

Both the left and right cutters in my previous reply were created as slot tools. only originally was I trying it as a custom tool. Only difference was after I created the slot tool, I then linked geometry from a level. Since the bottom section (arbor cap) wasn't set as cutter geometry I figured maybe mastercam would ignore it but that doesn't seem to be the case. 

I wonder how you could leave the cap simulated, but still perform these surface finishing toolpaths? if in the future the geometry wasn't so forgiving and I actually had to worry about the clearance.

thank you for all your help, and I hope I'm coming across clear enough.

22 minutes ago, danatoem said:

also flowline allows you to extend the cut motion off the part by using the "gap-settings" - "Tangential line length" !

wooooowww I love this forum haha, I always create a separate model, then model prep push/pull certain areas, then create surfaces from that solid, then chain to those surfaces,.. you just saved me a ton of future work, thank you.

 

18 minutes ago, Colin Gilchrist said:

Also, you can use "Direction" button to give you "surface lead in/out" motion, to get the tool in/out of the cut. For undercutting operations, you want to disable all of the "gouge checking" options.

this is also a great tip, I'll be fidgeting with these settings to see what kind of lead in/out I prefer. Thanks!

[JoshC]

15 minutes ago, Kyle F said:

Both the left and right cutters in my previous reply were created as slot tools. only originally was I trying it as a custom tool. Only difference was after I created the slot tool, I then linked geometry from a level. Since the bottom section (arbor cap) wasn't set as cutter geometry I figured maybe mastercam would ignore it but that doesn't seem to be the case. 

I wonder how you could leave the cap simulated, but still perform these surface finishing toolpaths? if in the future the geometry wasn't so forgiving and I actually had to worry about the clearance.

thank you for all your help, and I hope I'm coming across clear enough.

wooooowww I love this forum haha, I always create a separate model, then model prep push/pull certain areas, then create surfaces from that solid, then chain to those surfaces,.. you just saved me a ton of future work, thank you.

 

this is also a great tip, I'll be fidgeting with these settings to see what kind of lead in/out I prefer. Thanks!

here is an example with a custom tool that includes a nut at the bottom, just be aware the tool must still be touched off of the cutter portion and not the bottom of the nut from how this example was setup. nut.mcam

[Colin Gilchrist]

47 minutes ago, Kyle F said:

Both the left and right cutters in my previous reply were created as slot tools. only originally was I trying it as a custom tool. Only difference was after I created the slot tool, I then linked geometry from a level. Since the bottom section (arbor cap) wasn't set as cutter geometry I figured maybe mastercam would ignore it but that doesn't seem to be the case. 

I wonder how you could leave the cap simulated, but still perform these surface finishing toolpaths? if in the future the geometry wasn't so forgiving and I actually had to worry about the clearance.

thank you for all your help, and I hope I'm coming across clear enough.

wooooowww I love this forum haha, I always create a separate model, then model prep push/pull certain areas, then create surfaces from that solid, then chain to those surfaces,.. you just saved me a ton of future work, thank you.

 

this is also a great tip, I'll be fidgeting with these settings to see what kind of lead in/out I prefer. Thanks!

For "Direction", try setting the Plunge Angle to "0.0". (It will accept both positive and negative values! Try them both. Try a 5 degree ramp, and a -5 degree ramp, to see how it affects the entry/exit motion.)

Not all angles are created equal. It can be hard to tell "approach angle" and "exit angle" sometimes.

What I do is use a 1" entry distance, and a 2" exit distance, so I can then see "visually" based on the toolpath orientation, if I need to use a direction angle of 0-deg, 90-deg, 180-deg, or 270-deg, to get the "direction approach" I'm after.

Once I figure out the Plunge Angle, and Direction Angle settings, for both entry and exit, I will then adjust the actual distance to a reasonable value.

I'd also recommend changing your cut pattern to "zig-zag", and your Gap Method to "Smooth". Combining "Smooth" with "Tangent Line Extension" should give you an amazing cut pattern.

With one-way, if you insist on using it, you are better off making your "gap size just about double your step-over amount", and using the Tangent Line extension option. That would have you "cut through" each slice, beyond the surface, and then due to the gap distance (end of the last cut, to the start of the next cut) being greater than your Gap Size, the tool would then retract up to your Retract Plane, reposition to the start of the next cut slice, and cut through again.

[Kyle F]

43 minutes ago, JoshC said:

here is an example with a custom tool that includes a nut at the bottom, just be aware the tool must still be touched off of the cutter portion and not the bottom of the nut from how this example was setup. nut.mcam

Okay, I appreciate the clarification. So that was exactly as I had my tool setup, but once I imported geometry from a level, when the pop-up box asked if I wanted to override the previous blah blah, I said yes. So this time, I hit no, and voila! it worked. Thanks again, now everything is showing up perfect

 

20 minutes ago, Colin Gilchrist said:

For "Direction", try setting the Plunge Angle to "0.0". (It will accept both positive and negative values! Try them both. Try a 5 degree ramp, and a -5 degree ramp, to see how it affects the entry/exit motion.)

Not all angles are created equal. It can be hard to tell "approach angle" and "exit angle" sometimes.

What I do is use a 1" entry distance, and a 2" exit distance, so I can then see "visually" based on the toolpath orientation, if I need to use a direction angle of 0-deg, 90-deg, 180-deg, or 270-deg, to get the "direction approach" I'm after.

Once I figure out the Plunge Angle, and Direction Angle settings, for both entry and exit, I will then adjust the actual distance to a reasonable value.

I'd also recommend changing your cut pattern to "zig-zag", and your Gap Method to "Smooth". Combining "Smooth" with "Tangent Line Extension" should give you an amazing cut pattern.

With one-way, if you insist on using it, you are better off making your "gap size just about double your step-over amount", and using the Tangent Line extension option. That would have you "cut through" each slice, beyond the surface, and then due to the gap distance (end of the last cut, to the start of the next cut) being greater than your Gap Size, the tool would then retract up to your Retract Plane, reposition to the start of the next cut slice, and cut through again.

Excellent info! I love it. and I am not opposed to a zig zag pattern for the finish, my only worry is, I have never used a HSS convex radius cutter like this (only smaller carbide keyway tools from something like harvey tool) and I'm a little curious on how it would do in a conventional cut. 

sorry to get so deep into the weeds on this one haha

[crazy^millman]

2 hours ago, Kyle F said:

Excellent info! I love it. and I am not opposed to a zig zag pattern for the finish, my only worry is, I have never used a HSS convex radius cutter like this (only smaller carbide keyway tools from something like harvey tool) and I'm a little curious on how it would do in a conventional cut. 

sorry to get so deep into the weeds on this one haha

Speeds and feeds are extremely important when working with HSS. Remember the SFM is different at the 3" diameter verses the 2.625 diameter if that comes into contact at the very tangent of the radius. Use the 3" as the SFM process and go form there.