3D surfacing input/suggestion

Djstorm100 · Oct 4, 2020

First let me say I do not see a lot of 3D surfacing job and do not have a lot of experience with it. Over the weekend I took the time to play around with 3D surfacing.

While the finish is ok, it could be better

Machines Haas vf2ss 2019
Material 6061

Operations
Rough with 1/2” to get the step stair look leaving 0.020 radial and axially

Came in with roughing parallel tool path 3/8 ball nose. Step over is 0.030 leaving 0.005 axially. IPM 150, 10k rpm, 0.005IPT

Finishing is same ball nose 0.005 doc step over is 0.005 (left part in the below picture, 0.010 step over on the right. 0.010 i want to say was feed rate of 175ipm) 225ipm. I can’t remember rpm but the effective chip thickness is 0.0006. 8,000 rpm, 225IPM.

The tool was moving back and forth in XZ zigzagging. The surface is smooth, if you run your finger nail over the surface fast enough you can hear it make a ripple type sound. Sorry if I’m explaining that wrong.

I’m thinking why the surface finish looks the way it does is from chip thickness being so low due to chip thinning? Thought? Thanks in advance

The 3D chamfer came out great
**Finish ball end mill** Notice the actual chip thickness is 0.0007 I went faster to make a better chip.

Sent from my iPhone using Tapatalk

Delw · Oct 4, 2020

Djstorm100 said:
First let me say I do not see a lot of 3D surfacing job and do not have a lot of experience with it. Over the weekend I took the time to play around with 3D surfacing.

While the finish is ok, it could be better

Machines Haas vf2ss 2019
Material 6061

Operations
Rough with 1/2” to get the step stair look leaving 0.020 radial and axially

Came in with roughing parallel tool path 3/8 ball nose. Step over is 0.030 leaving 0.005 axially. IPM 175

Finishing is same ball nose 0.005 doc step over is 0.005 (left part in the below picture, 0.010 step over on the right. 0.010 i want to say was feed rate of 175ipm) 225ipm. I can’t remember rpm but the effective chip thickness is 0.0006

The tool was moving back and forth in XZ zigzagging. The surface is smooth, if you run your finger nail over the surface fast enough you can hear it make a ripple type sound. Sorry if I’m explaining that wrong.

I’m thinking why the surface finish looks the way it does is from chip thickness being so low due to chip thinning? Thought? Thanks in advance

The 3D chamfer came out great

Sent from my iPhone using Tapatalk

feed rates way to fast, cut it down to 100IPM maybe 125IPM running 12krpm
I used to primarily only do surfacing on my fadal and hass, with that 3/8s ball you might be able to run a step over of .010 and get a smooth finish at slower IPM but may have to drop it to .007 or even .005 step over. BTW if your running the opposite direction of the angle you'll need to run 50% less step over.

meowkat · Oct 4, 2020

Djstorm100 said:
First let me say I do not see a lot of 3D surfacing job and do not have a lot of experience with it. Over the weekend I took the time to play around with 3D surfacing.

While the finish is ok, it could be better

Machines Haas vf2ss 2019
Material 6061

Operations
Rough with 1/2” to get the step stair look leaving 0.020 radial and axially

Came in with roughing parallel tool path 3/8 ball nose. Step over is 0.030 leaving 0.005 axially. IPM 175

Finishing is same ball nose 0.005 doc step over is 0.005 (left part in the below picture, 0.010 step over on the right. 0.010 i want to say was feed rate of 175ipm) 225ipm. I can’t remember rpm but the effective chip thickness is 0.0006

The tool was moving back and forth in XZ zigzagging. The surface is smooth, if you run your finger nail over the surface fast enough you can hear it make a ripple type sound. Sorry if I’m explaining that wrong.

I’m thinking why the surface finish looks the way it does is from chip thickness being so low due to chip thinning? Thought? Thanks in advance

The 3D chamfer came out great

[...]

Sent from my iPhone using Tapatalk

It looks like the classic ball nose effect, using too much of the very point of the ball. I'm sure you already know this, but a corner radius endmill would probably leave a better finish.

macds · Oct 5, 2020

Ball mill effect, yes.
Why was XY zigzagging? That looks rough to me.

I do a lot of ball mill surfacing, something isnt right there. Feed rate is part of it, since thats a very shallow angle.

Djstorm100 · Oct 5, 2020

meowkat said:
It looks like the classic ball nose effect, using too much of the very point of the ball. I'm sure you already know this, but a corner radius endmill would probably leave a better finish.

This is what I'm leading to believe. I saw a friends picture on instagram and got me thinking, granted he used 1/2" vs 3/8" and was 4140 vs 6061. His surface is better.

Delw said:
feed rates way to fast, cut it down to 100IPM maybe 125IPM running 12krpm
I used to primarily only do surfacing on my fadal and hass, with that 3/8s ball you might be able to run a step over of .010 and get a smooth finish at slower IPM but may have to drop it to .007 or even .005 step over. BTW if your running the opposite direction of the angle you'll need to run 50% less step over.

I was running 8,000 rpm 225 ipm to help generate a thicker chips. I shot my self in the toe by leaving so little stock (0.005). Had I left more, I could of slowed the rpm down and ipm to still hit 0.001 actual chip. I try to make a 0.001 chip to help prevent rub.

macds said:
Ball mill effect, yes.
Why was XY zigzagging? That looks rough to me.

I do a lot of ball mill surfacing, something isnt right there. Feed rate is part of it, since thats a very shallow angle.

If I only went one way, the cycle time increased about 5x.
Below is tool engagement. This is at 0.010 doc and 0.010 step over.

Mike1974 · Oct 5, 2020

Zig zag should be fine. What other options do you have for surfacning? I like constant stepover/scallop. Not sure how much it will affect fit/finish, but sometimes it makes a pretty big difference on one or the other, sometimes both.

aarongough · Oct 5, 2020

For this part, given that it's only flat areas or shallow angles, no place where the tool needs to make large sudden changes in Z, as already said a corner radius tool will leave a MUCH better finish.

When cutting shallow surfaces like this with a ball nose you end up mainly just using the very tip of the tool, which has a really small effective diameter, and usually only a single cutting flute. Even on high flute count ballnose tools there is usually only a single cutting edge that crosses over the center of the tip to make it 'center cutting'. These two factors combined mean that when you're cutting shallow/flat surfaces with a ball-nose you end up 'smearing' the material rather than actually cutting it, which in turn makes the finish look like crap.

Personally if I was tackling this part here is how I would handle it:

I would divide the part into two toolpaths, one to finish the flat top area with a wider stepover, and another that uses a corner radius tool to finish the angled areas. Both toolpaths would be parallel finishing toolpaths cutting both ways provided that leaves acceptable finish.

Your 0.005" stepover would be fine for the angled areas, with a large corner radius that will leave a really nice finish. Finishing the flat area separately with a larger stepover will save you a LOT of cycle time. Something like .125" for the top surface would work.

Use the largest tool you can with a nice big corner radius. Something like this 5/8" 3 flute with .125" corner rad would be perfect: 5/8 3 Flute Carbide End Mill SE 38 Deg Helix 1.625 LOC With .125 corner Radius MariTool

Make sure you use the same tool/toolholder to finish the top and the angles so there is no issue blending the toolpaths together! Set the top surface as a 'do not touch' surface when creating the toolpaths for the angled areas to make sure it doesn't gouge.

A setup like that should get you beautiful finishes... The only caveat being that the finish on the top is going to look slightly different to the finish on the angles because you're using different parts of the tool. You could minimize that by doing everything with the same stepover, but obviously that will cost cycle time...

Djstorm100 · Oct 5, 2020

aarongough said:
For this part, given that it's only flat areas or shallow angles, no place where the tool needs to make large sudden changes in Z, as already said a corner radius tool will leave a MUCH better finish.

When cutting shallow surfaces like this with a ball nose you end up mainly just using the very tip of the tool, which has a really small effective diameter, and usually only a single cutting flute. Even on high flute count ballnose tools there is usually only a single cutting edge that crosses over the center of the tip to make it 'center cutting'. These two factors combined mean that when you're cutting shallow/flat surfaces with a ball-nose you end up 'smearing' the material rather than actually cutting it, which in turn makes the finish look like crap.

Personally if I was tackling this part here is how I would handle it:

I would divide the part into two toolpaths, one to finish the flat top area with a wider stepover, and another that uses a corner radius tool to finish the angled areas. Both toolpaths would be parallel finishing toolpaths cutting both ways provided that leaves acceptable finish.

Your 0.005" stepover would be fine for the angled areas, with a large corner radius that will leave a really nice finish. Finishing the flat area separately with a larger stepover will save you a LOT of cycle time. Something like .125" for the top surface would work.

Use the largest tool you can with a nice big corner radius. Something like this 5/8" 3 flute with .125" corner rad would be perfect: 5/8 3 Flute Carbide End Mill SE 38 Deg Helix 1.625 LOC With .125 corner Radius MariTool

Make sure you use the same tool/toolholder to finish the top and the angles so there is no issue blending the toolpaths together! Set the top surface as a 'do not touch' surface when creating the toolpaths for the angled areas to make sure it doesn't gouge.

A setup like that should get you beautiful finishes... The only caveat being that the finish on the top is going to look slightly different to the finish on the angles because you're using different parts of the tool. You could minimize that by doing everything with the same stepover, but obviously that will cost cycle time...

Thank you and the rest of you guys. I'll run the part again with the suggested tool. The whole top is angled (3 different angles)

aarongough · Oct 5, 2020

Djstorm100 said:
The whole top is angled (3 different angles)View attachment 301197

Ah! Didn't realize that from the first photo, makes sense!

Please post back and let us know how it goes!

Some of the other guys might have more info that is specific to aluminum, I don't run much aluminum, mainly hardened tool steels...

EDIT: Also, that is going to be a really cool looking part when it's done! Definitely want follow-up pics!

Djstorm100 · Oct 5, 2020

aarongough said:
Ah! Didn't realize that from the first photo, makes sense!

Please post back and let us know how it goes!

Some of the other guys might have more info that is specific to aluminum, I don't run much aluminum, mainly hardened tool steels...

EDIT: Also, that is going to be a really cool looking part when it's done! Definitely want follow-up pics!

Thank you. The issue I'm fighting with my self feed and speed. I'm a familiar believer to try and make at least 0.001 chip with anything 1/8 and above. WOC dictates the chip thickness.

This is with bullnose 1/2" with 0.125 raidus.
DOC .020 WOC .010 @ 12,000 RPM W/ 0.005 IPT is 204 ipm= to actual chip thickness of 0.001 due to chip thinning.

Finegrain · Oct 5, 2020

Djstorm100 said:
Thank you. The issue I'm fighting with my self feed and speed. I'm a familiar believer to try and make at least 0.001 chip with anything 1/8 and above. WOC dictates the chip thickness.

DOC .020 WOC .010 @ 12,000 RPM W/ 0.005 IPT is 204 ipm= to actual chip thickness of 0.001 due to chip thinning.

Your chip thinning calc is off I think. Since your ball endmill is only cutting at the very tip, it's as if you were running a 1/16" or 1/8" endmill. Chip thinning at those diameters is going to be much less of a factor than at 1/2".

Regards.

Mike

TheBigLebowski · Oct 5, 2020

As everyone else has said, the SFM at the tip of a ballnose is effectively 0, so you will never get a great finish on a 3x when the part is near flat.

Do you have a quantity of these to make or just a single part? If you are making more then a single part, you could build a fixture to tilt the part up so you can just mill the top part as a flat plane, this would probably cut your cycle time down by 5-10x.

Depending on how accurate you need the part to be, you could also run the same toolpath with a bullnose and get a better finish, But beware that some bullnose cutters have corners that are not all that accurate.

if you have any lines that seem a little deeper then the rest, you can try a zigzag (parallel milling in both directions) in the xy direction instead of xz. this way you just have single axis motion instead of coordinated xz motion. technically speaking it should be more accurate.

mhajicek · Oct 5, 2020

Don't worry about chip thinning with finish passes; that's for roughing. In aluminum, especially with a ball endmill, you should be running at max RPM. 30K RPM would not be too fast. The tip of your 3 flute endmill probably only has one cutting flute at the center, so figure based on that how big you want those scallops to be; that's your chipload per revolution. As said above, a larger bull (corner radius) endmill, moving along the surface in the up/down direction, will do much better. I once surfaced a slight incline with a 4" face mill and .050" stepover; the finish was beautiful.

Djstorm100 · Oct 5, 2020

Finegrain said:
Your chip thinning calc is off I think. Since your ball endmill is only cutting at the very tip, it's as if you were running a 1/16" or 1/8" endmill. Chip thinning at those diameters is going to be much less of a factor than at 1/2".

Regards.

Mike

Mike, my apolgoize the above was with a 1/2 bull nose (.125 radius) not with the ball nose

TheBigLebowski said:
As everyone else has said, the SFM at the tip of a ballnose is effectively 0, so you will never get a great finish on a 3x when the part is near flat.

Do you have a quantity of these to make or just a single part? If you are making more then a single part, you could build a fixture to tilt the part up so you can just mill the top part as a flat plane, this would probably cut your cycle time down by 5-10x.

Depending on how accurate you need the part to be, you could also run the same toolpath with a bullnose and get a better finish, But beware that some bullnose cutters have corners that are not all that accurate.

if you have any lines that seem a little deeper then the rest, you can try a zigzag (parallel milling in both directions) in the xy direction instead of xz. this way you just have single axis motion instead of coordinated xz motion. technically speaking it should be more accurate.

I'm just doing these as test pieces, learning and experience really

macds · Oct 5, 2020

Djstorm100 said:
This is what I'm leading to believe. I saw a friends picture on instagram and got me thinking, granted he used 1/2" vs 3/8" and was 4140 vs 6061. His surface is better.

View attachment 301185

I was running 8,000 rpm 225 ipm to help generate a thicker chips. I shot my self in the toe by leaving so little stock (0.005). Had I left more, I could of slowed the rpm down and ipm to still hit 0.001 actual chip. I try to make a 0.001 chip to help prevent rub.

If I only went one way, the cycle time increased about 5x.
Below is tool engagement. This is at 0.010 doc and 0.010 step over.
View attachment 301186

Gotcha now.... i wasnt understanding what you were saying.

A soft material is generally going to leave a poor surface finish when ball contouring on low angles, as the core of the mill is more smearing the material out of the way.... doesnt matter what the diameter of ball is.
4140PH is going to be a lot more forgiving.

As crazy as it sounds, youll get a better finish on flats (low angle curved surfaces) using a little dinky endmill, as the engagement scallop ends up further up the radius.

Now, if you want a really nice surface finish on flats using a ball, and you have nothing standing on the part that will interfere, toss a tooling ball on the part for location, and tip it up on 20 degrees.....

Delw · Oct 6, 2020

Djstorm100 said:
I was running 8,000 rpm 225 ipm to help generate a thicker chips. I shot my self in the toe by leaving so little stock (0.005). Had I left more, I could of slowed the rpm down and ipm to still hit 0.001 actual chip. I try to make a 0.001 chip to help prevent rub.

Sometimes we gotta learn not to rely on the "BOOK/CHIP LOAD" so to speak. I surfaced on a old Acroloc with a 6k spindle for years we got 63 finishes no problem. if I recall it was with 1/4 2 flute ball endmills running maybe 35-40IPM.

but aside from speeds and feeds, there are other things that are important to surfacing while most will agree that step over is very critical, you also have to look at how long your line segment is. That will definatey effect the finish quality doing a zigzag path and machines that dont have high speed machining.
When we got our 2009 hass vf2ss they came in and set it up I had the highspeed machining option. the finished looked like trash. no matter what we tried it was really bad. called the factory cause the locals couldnt figure it out and they had me changes some PRMS after a few tries and few different changes parts looked really nice.
I don't remember the exact prm numbers or there settings but maybe one of the Guys here on the board will have an idea which ones. if not I can look if need be.

generally I will leave .010 stock for surfacing if I have a profile tolorance off less that .005 all over I will run a semi finish to .003 then run a finish pass.
this is on alum as well as everything else ( we mainly did alum, but done a bunch of big heical gears 9310- 4340 etc etc that wouldnt fit in my buddies gear machines. generally for surfacing we use 1/8 and smaller due to fillet rads we need to hold. about 3/64 balls are the smallest I have gone. if you have fillet or sharp angles to surface thats where you need to cut your step over in have at a absolute min.

Dont know what kinda software you have but next time your playing around run a steep angle into a fillet with a step over of lets say .010 and look at the line spacing compared to the flats and the angles and fillets. Surfacing to be successful takes some time to get used to before you know it you wont have to test anymore just program hit the green button and your parts will be perfect.

Hardplates · Oct 6, 2020

I would definitely use a bullnose for what you are trying to do. You are also wasting a ton of time cutting air when you are going over the pockets.

When doing 3D surfacing you can often throw chipload calcs out the window. At the end of the day surface finish is what matters.

Depending on your machines capabilities you may not be able to zig zag and have to only zig (only cut in one direction)

Djstorm100 · Oct 6, 2020

Delw said:
Sometimes we gotta learn not to rely on the "BOOK/CHIP LOAD" so to speak. I surfaced on a old Acroloc with a 6k spindle for years we got 63 finishes no problem. if I recall it was with 1/4 2 flute ball endmills running maybe 35-40IPM.

but aside from speeds and feeds, there are other things that are important to surfacing while most will agree that step over is very critical, you also have to look at how long your line segment is. That will definatey effect the finish quality doing a zigzag path and machines that dont have high speed machining.
When we got our 2009 hass vf2ss they came in and set it up I had the highspeed machining option. the finished looked like trash. no matter what we tried it was really bad. called the factory cause the locals couldnt figure it out and they had me changes some PRMS after a few tries and few different changes parts looked really nice.
I don't remember the exact prm numbers or there settings but maybe one of the Guys here on the board will have an idea which ones. if not I can look if need be.

generally I will leave .010 stock for surfacing if I have a profile tolorance off less that .005 all over I will run a semi finish to .003 then run a finish pass.
this is on alum as well as everything else ( we mainly did alum, but done a bunch of big heical gears 9310- 4340 etc etc that wouldnt fit in my buddies gear machines. generally for surfacing we use 1/8 and smaller due to fillet rads we need to hold. about 3/64 balls are the smallest I have gone. if you have fillet or sharp angles to surface thats where you need to cut your step over in have at a absolute min.

Dont know what kinda software you have but next time your playing around run a steep angle into a fillet with a step over of lets say .010 and look at the line spacing compared to the flats and the angles and fillets. Surfacing to be successful takes some time to get used to before you know it you wont have to test anymore just program hit the green button and your parts will be perfect.

I have HSM on my machine, it does work great so far. The 3d Chamfer (scallop tool path w/ 3/8 ball) turned out great. I use Fusion 360.

Hardplates said:
I would definitely use a bullnose for what you are trying to do. You are also wasting a ton of time cutting air when you are going over the pockets.

When doing 3D surfacing you can often throw chipload calcs out the window. At the end of the day surface finish is what matters.

Depending on your machines capabilities you may not be able to zig zag and have to only zig (only cut in one direction)

That's kind of a problem, how is one suppose to calculate feed. It did some zig zagging on a 3d chamfer and that turned out very well. The finish on the surface of the part is uniform and smooth. I just know it can be better.

I've got a 1/2" dia EM with a 0.125 radius.

Hardplates · Oct 6, 2020

Djstorm100 said:
That's kind of a problem, how is one suppose to calculate feed. It did some zig zagging on a 3d chamfer and that turned out very well. The finish on the surface of the part is uniform and smooth. I just know it can be better.

I've got a 1/2" dia EM with a 0.125 radius.

Program a test piece with some different feeds. Don't be afraid to play with the override knobs. Do it enough and you'll get a feel for where you need to be just by looking at a model.

I try to only use balls when I have to get into a corner or want to take a large stepdown on steep slopes. Like many have said here the center of the tool isn't cutting cause it's not "moving"

Different machines can surface at different speeds, best to start slow and work your way up till it stops following the toolpath. 200 ipm is moving right along even for a die and mold type machine.

Mike1974 · Oct 6, 2020

Hardplates said:
I would definitely use a bullnose for what you are trying to do. You are also wasting a ton of time cutting air when you are going over the pockets.

When doing 3D surfacing you can often throw chipload calcs out the window. At the end of the day surface finish is what matters.

Depending on your machines capabilities you may not be able to zig zag and have to only zig (only cut in one direction)

Maybe, maybe not. Sometimes saving programming time can justify the air cutting. Or depending on processing power of machine and cam, could take longer/the same even though less cutting moves if the machine is jerking around "dodging" (

) the pocket areas.

3D surfacing input/suggestion

Cast Iron

Attachments

Stainless

Aluminum

Hot Rolled

Cast Iron

Attachments

Diamond

Stainless

Cast Iron

Stainless

Cast Iron

Diamond

Aluminum

Diamond

Cast Iron

Hot Rolled

Stainless

Stainless

Cast Iron

Stainless

Diamond

Similar threads