What's new
What's new

Help with 3d toolpath surface finish and speeds?

OliviaB

Plastic
Joined
Nov 30, 2023
Hey all.

I'm making a part out of some 17-4 H900 SS. The feature I'm concerned about is a .850" diameter boss with a 2" radius on the top of it, similar to a section cut out of a hemisphere. I'm looking for a good surface finish here, but I'm also not looking to wait 20 hours for my machine to run through the program. I wrote the toolpaths a week ago, and looking at them again, I'm unsure if my numbers are gonna work

The tool i have to use for this feature is a 1/16" end mill. I have a Harvey 6fl stub long reach cutter that i picked out. My machine is a small toolroom style 3 axis, which caps at 6k rpm, 100ipm. There is .002 stock left for the finish tool to come in. I only have one finishing tool, and don't have a lot of room for experimenting.

I've been told that for a good 3d surface finish, one must match the IPT to the stepover. I currently have it setup for a .0001 scallop height, an my stepover will be around .0027. If I set my IPT to this same number, I'll be running at around 97 IPM which just feels insane for this material. I know that radial chip thinning exists, but I honestly am not sure how to apply it to this. Do these numbers sound okay?

Any tips would be much appreciated, I am the only CNC person in my shop so I have nowhere else to turn for advice. Thanks in advance!
 
Last edited:
Why do you have to use such a small cutter?
Since its a convex feature you should be able to run a much larger tool = not going to feel so hamstrung by your low RPM, and you can get away with a larger stepover.
Im stuck using such a small cutter because taller features are at such close proximity. The nearest feature is .072 away, and to hit all of the geometry, my end mill has to fit into this space
 
yes, but you don't need to cut the whole thing with a 1/16" tool. Use a large tool, then swap to the small tool only when you need it.
That’s a good point. I’ll try that. Still, I’m having a hard time figuring out my speeds and feeds
 
Your stepover looks fine, with that low of an RPM limit I'd probably be at 20ipm for a good finish with that tool. I'd try that and see how it looks and then adjust. And like others have said use an 1/8" ball or larger for as much as you can.
 
That’s a good point. I’ll try that. Still, I’m having a hard time figuring out my speeds and feeds
Go download HSMAdvisor for speeds/feeds.

Post a pic of your part so the brain trust can offer better advice.
 
Your stepover looks fine, with that low of an RPM limit I'd probably be at 20ipm for a good finish with that tool. I'd try that and see how it looks and then adjust. And like others have said use an 1/8" ball or larger for as much as you can.

1/16 endmill at 20ipm, really? That wouldn't last but a few seconds

I'd think 1-1.5in/min max
 
Go download HSMAdvisor for speeds/feeds.

Post a pic of your part so the brain trust can offer better advice.

Here's the feature
1707912843387.png
Admittingly, I am limited by my Mastercam license to only use single surface flowline toolpaths, because my company wont invest in mill 3d.

I've already made one part out of A2, but was unhappy with my surface finishes.
 
1/16 endmill at 20ipm, really? That wouldn't last but a few seconds

I'd think 1-1.5in/min max

LOL.

My friend, what a luxury it would be to run that slowly.


To the OP. Feeds and speeds are readily available in the catalog for the tool. It doesn’t have to be a guessing game. Start at the recommended feed, and then crank it up as you reduce step over.
 
LOL.

My friend, what a luxury it would be to run that slowly.


To the OP. Feeds and speeds are readily available in the catalog for the tool. It doesn’t have to be a guessing game. Start at the recommended feed, and then crank it up as you reduce step over.

Harvey catalog

.00012"*6fl*6000rpm = 4.32ipm

the OP is going to be plunging down faces. That's probably where their going to be breaking endmills.

-----------------------------------

Fuck it run it 20ipm.

That'll be fun watching when it goes down faces (flowlines remember)
 
LOL.

My friend, what a luxury it would be to run that slowly.


To the OP. Feeds and speeds are readily available in the catalog for the tool. It doesn’t have to be a guessing game. Start at the recommended feed, and then crank it up as you reduce step over.
I ran their recomended feeds and speeds for the majority of the part. I was under the assumption that if its only cutting .002 of stock than I could turn my feeds way up
 
If your nearest feature is .072 away thats more than the radius of a 1/8 endmill. Use the bigger endmill please. Also, stubbier the better.
I will definitely switch to a 1/8 for the majority of it. I'll just need to use my 1/16" to achieve the needed corner radius. What was really stopping me from trying this, was leaving a visible surface mismatch. Though, I would prefer a mismatch over 6 hours of flowline feed time
 
Harvey catalog

.00012"*6fl*6000rpm = 4.32ipm

the OP is going to be plunging down faces. That's probably where their going to be breaking endmills.

-----------------------------------

Fuck it run it 20ipm.

That'll be fun watching when it goes down faces (flowlines remember)
Running tools this small has me tensed up regardless of the operation, ive already broken two of them with stupid little programming errors
 
20 IPM is pretty aggressive for a 1/16 ball in SS regardless of having very little stock leftover.

I'd hit the top surface with a 1/8 ball, flow outside to in, .002 or .003 stepover maximum. That tool you might program for 20 or 25 IPM. Also, don't know what kind of mill you have but from the sounds of it if I were you I'd change the cut tolerances. Go into flowline parameters, on finish flowline parameters click the "total tolerance" button. Check the line/arc filtering settings to on, then up above change your cut tolerance to 30% (if you haven't already). This ought to give you smoother motion and a help on your surface finish.

Walk down the top corner radius and walls with the 1/16 ball, that's gonna be more in line with what @triumph406 said. I'd send that to the floor with all the same cut tolerance parameters set up, max RPM at 8 IPM at the absolute highest. I'm guessing on the floor it's probably getting changed to 5 or 6 IPM.
 
Running tools this small has me tensed up regardless of the operation, ive already broken two of them with stupid little programming errors

Well if your an employee, and the company pays for the tools. Who cares?

If your on your own (like me) breaking tools could get to be a problem

-----------------------------------

Get used to breaking tools, small programming errors are inevitable, especially when starting out.

Even after running decades like myself I still make stupid mistakes. But then I'm the exception, most here are perfect and never make mistakes 😂
 








 
Back
Top