[CadRhino]

Hi Fellow Tormachers,

I am making a run of these parts in 6061 aluminum and I am not really happy with my finish results so far.
The non-corner rounded part is held .2" deep in a vise very snugly and the corner rounded side is held .5" deep very firmly in a vise.
As you can see from the photos, there are lots of tiny vertical lines left over from the cutters.
Here is what I am using;
1) Main cutting (on vertical sides) is a Tormach 1/4" HSS E.M. in an ER20 collet at 5100 RPM and 12 IPM.
2) Chamfering is done with Maritool 1/4" 4-flute carbide cutter in 1/4" dia. tool holder 5100 RPM and 12 IPM.
3) Corner round is done with Maritool .187 radius 4-flute carbide cutter in 1/2" dia. tool holder running at 5100 RPM and 5 IPM.

I originally cut the corner round at 5100 RPM and 12 IPM but it had the same line issue so I reduced the feed to 5 IPM and it is better but as you can see it still has a bunch of small vertical lines from the cutter.

Any thoughts on what might be happening or how I can get a better finish? Change the speeds/Feeds?
If just one of the tools was having this issue I would think it was that particular tool but all of the tools are creating these lines in surface finish.

I have some Lake Shore carbide 1/4" 2-flute EM's coming to see if they are better but I need to stick with the MariTool profile cutters for now.

Thanks,
Nathan

[SCzEngrgGroup]

Have you tried taking multiple finish passes, including a final "spring pass"?

Regards,
Ray L.

[CadRhino]

Hi Ray,

Only on the corner round did I do a finish pass of .003" and I still have those lines.

Good suggestion (I should have done it on the rest of the ops but they are not visible).

I was just expecting overall better finish.

I will add a .003" finish pass to the other ops and that will probably help but I suspect I will still get the lines (just finer).

Thanks,

-Nathan

Have you tried taking multiple finish passes, including a final "spring pass"?

Regards,
Ray L.

[popspipes]

Machine marks will always be present, they get smaller with lower feedrates but never completely go away as they are a function of the cutting action of the cutter.
I always take a finish pass on everything of .005 to .01, it does improve the finish.
I also have a vibrator finisher with walnut hulls and emery grit mixed with it that works to brighten parts up,

I finish at 5140 rpm and 20 to 35 feedrate but the spindle and drive are balanced pretty well so the finish is better but I still have the marks, they are just more even.

I also use 4 flute cutters for finishing.

[pickled]

Agreed with the comments above. The other piece to verify is that you are at the shortest stick-out of the tool that you can get for your set-up. I typically only give my tools a reserve of about 0.015" in length to get a high finish job done. Expensive carbide tooling is nicer in this regard, but it even likes to be choked up a bit in the holders. Your radius cutter did quite well and a little bit of hand finish or walnut lovin' should make that area shine. What DOC were you using for your chamfer and how high was your contact point?

[MichaelHenry]

To me, it would be a lot easier (and faster) to get a good finish on parts like that with a lathe, either CNC or manual. If a dull matte finish, rather than bright, is acceptable than you might try tumbling the mill-machined parts.

Mike

On edit: Using the Tormach as a lathe, as others here have shown, might also be a good solution.

[G59]

You should try a 3 flute endmill. This was discussed in another thread how the spindle harmonics affect finish. The 3 flutes create their own harmonics but at different frequencies. This difference in frequency can sometimes dampen or even cancel each other out eliminating tool marks.

[SCzEngrgGroup]

Hi Ray,

Only on the corner round did I do a finish pass of .003" and I still have those lines.

Good suggestion (I should have done it on the rest of the ops but they are not visible).

I was just expecting overall better finish.

I will add a .003" finish pass to the other ops and that will probably help but I suspect I will still get the lines (just finer).

Thanks,

-Nathan

Try taking a heavier finish pass. At 0.003", you may be rubbing. Cutting tools like to have a good "bite", and will often cut better when working harder. My typical finish cut is 0.01". Try both slowing down, and speeding up, feedrate. Depending on conditions, either one can improve finish.

I don't know what the quality of the Tormach endmills is, but the specific tool makes a HUGE difference. Those may simply not be very good endmills.

Regards,
Ray L.

[kfriedrich66]

Try taking a heavier finish pass. At 0.003", you may be rubbing. Cutting tools like to have a good "bite", and will often cut better when working harder. My typical finish cut is 0.01". Try both slowing down, and speeding up, feedrate. Depending on conditions, either one can improve finish.

I don't know what the quality of the Tormach endmills is, but the specific tool makes a HUGE difference. Those may simply not be very good endmills.

Regards,
Ray L.

Umm this contradicts your "spring pass" suggestion earlier which would be removing a minute amount of material and more than likely leave a worse finish.

Nathan, are you using a finishing endmill, 4 flutes or better for your finish work?
Kate

[G59]

Taking a 0.01 cut can be beneficial as a final pass, as you are biting into the material instrad of rubbing it off. A lot of it depends on the quality of the cutter.

[Steve Seebold]

Hi Fellow Tormachers,

I am making a run of these parts in 6061 aluminum and I am not really happy with my finish results so far.
The non-corner rounded part is held .2" deep in a vise very snugly and the corner rounded side is held .5" deep very firmly in a vise.
As you can see from the photos, there are lots of tiny vertical lines left over from the cutters.
Here is what I am using;
1) Main cutting (on vertical sides) is a Tormach 1/4" HSS E.M. in an ER20 collet at 5100 RPM and 12 IPM.
2) Chamfering is done with Maritool 1/4" 4-flute carbide cutter in 1/4" dia. tool holder 5100 RPM and 12 IPM.
3) Corner round is done with Maritool .187 radius 4-flute carbide cutter in 1/2" dia. tool holder running at 5100 RPM and 5 IPM.

I originally cut the corner round at 5100 RPM and 12 IPM but it had the same line issue so I reduced the feed to 5 IPM and it is better but as you can see it still has a bunch of small vertical lines from the cutter.

Any thoughts on what might be happening or how I can get a better finish? Change the speeds/Feeds?
If just one of the tools was having this issue I would think it was that particular tool but all of the tools are creating these lines in surface finish.




I have some Lake Shore carbide 1/4" 2-flute EM's coming to see if they are better but I need to stick with the MariTool profile cutters for now.

Thanks,
Nathan

You're just running the spindle too fast. I get a great finish on my PCNC 1100 Series II. I have experimented with feeds and seeds with my machine since I got it in July 2011. I learned that at 5100 RPM, the finish on both the walls and the floor sucks, but if I leave .015 to .025 on the floor and walls for a finish cut, use a 3/8 3 flute end mill and reduce spindle speed to 3500 RPM at 25 to 30 IPM I will get a beautiful finish.

[CadRhino]

Hi Popspipes,
Thanks for the insight.
I have a Harbor Freight vibrator I have not used yet so this may be a good reason to get it set up.
What kind of Walnut shell and grit do you use and where do you get it?
Thanks for the feedback on feeds and using a 4 flute for finish passes. I have 2 flute beaten into my head for aluminum but that makes sense.
Best,
Nathan

Machine marks will always be present, they get smaller with lower feedrates but never completely go away as they are a function of the cutting action of the cutter.
I always take a finish pass on everything of .005 to .01, it does improve the finish.
I also have a vibrator finisher with walnut hulls and emery grit mixed with it that works to brighten parts up,

I finish at 5140 rpm and 20 to 35 feedrate but the spindle and drive are balanced pretty well so the finish is better but I still have the marks, they are just more even.

I also use 4 flute cutters for finishing.

[CadRhino]

I had the chamfer up .02" and added another fudge factor of .02" stock to the chamfer so it was .03" up from the tip of the chamfer tool. I use sprutcam so that is the formula I used so it was not cutting on the tip.

Agreed with the comments above. The other piece to verify is that you are at the shortest stick-out of the tool that you can get for your set-up. I typically only give my tools a reserve of about 0.015" in length to get a high finish job done. Expensive carbide tooling is nicer in this regard, but it even likes to be choked up a bit in the holders. Your radius cutter did quite well and a little bit of hand finish or walnut lovin' should make that area shine. What DOC were you using for your chamfer and how high was your contact point?

[CadRhino]

Agreed but I am going to be doing quite a bit of work on the back sides and I only have a manual lathe which I am not terribly fast on.

To me, it would be a lot easier (and faster) to get a good finish on parts like that with a lathe, either CNC or manual. If a dull matte finish, rather than bright, is acceptable than you might try tumbling the mill-machined parts.

Mike

On edit: Using the Tormach as a lathe, as others here have shown, might also be a good solution.

[CadRhino]

Thanks G59.
I actually have a 3-flute roughing E.M. I bought from tormach and will try it.

You should try a 3 flute endmill. This was discussed in another thread how the spindle harmonics affect finish. The 3 flutes create their own harmonics but at different frequencies. This difference in frequency can sometimes dampen or even cancel each other out eliminating tool marks.

[CadRhino]

Hi Kate,
I am using the same tool for rough and finish so I am not switching over to a 4fl for finish but I will do that.
It is the chamfering and corner rounding that is getting me. Those are 4 flute and I was hoping for a better (mirror) finish but maybe, like popspipes said, it will always have some lines.
Ray's, comments kind of mesh with what Frank Mari (Mari tools) told me today. He said I might want to try 2000 rpm and 30 IPM and mix it up. That my machine might be having a funny 'harmonics' at 5100 RPM and that I might want to find the sweat spot for each too.
Best,
Nathan

Umm this contradicts your "spring pass" suggestion earlier which would be removing a minute amount of material and more than likely leave a worse finish.

Nathan, are you using a finishing endmill, 4 flutes or better for your finish work?
Kate

[CadRhino]

Thanks Ray.
I will mix it up and try it.
I also have a 3/8" Tool 3/FL finishing rougher I should test as well.

You're just running the spindle too fast. I get a great finish on my PCNC 1100 Series II. I have experimented with feeds and seeds with my machine since I got it in July 2011. I learned that at 5100 RPM, the finish on both the walls and the floor sucks, but if I leave .015 to .025 on the floor and walls for a finish cut, use a 3/8 3 flute end mill and reduce spindle speed to 3500 RPM at 25 to 30 IPM I will get a beautiful finish.

[SCzEngrgGroup]

Umm this contradicts your "spring pass" suggestion earlier which would be removing a minute amount of material and more than likely leave a worse finish.

Nathan, are you using a finishing endmill, 4 flutes or better for your finish work?
Kate

The point, is, you have to try different things. There are countless factors that can affect finish quality, and some can only be found by experimentation. Feeds and speeds that work well on one machine, may be awful on another, due to small differences in the cutting tool geometry, or machine or tool resonances. Even a small change in RPM can sometimes have a large effect. But, in general, tools are happier with a higher chipload. That can be achieved by reducing RPM, or increasing feedrate. If all is perfect, a spring pass can help, otherwise, it might hurt. You just have to experiment, and find what works best for you, with your tool, on your machine. For me, 3-flute tools are rarely an improvement. For others, they are. I also generally get better finish with a 2-flute than with a 4- or even 6-flute. Go figure...

Regards,
Ray L.

[LeeWay]

I put this video in the other thread that was mentioned.
https://www.youtube.com/watch?v=9eyA2kq7lDM

It is a home made mill that has worked great for me. Finish passes should be very slow to take out some of the resonance and frequency issues. These parts off this little machine were pro quality. Almost mirror finish. The pictures do not do those parts justice. That is the result you are looking for. Something like a FINISHED part.

[SCzEngrgGroup]

Hi Popspipes,
Thanks for the insight.
I have a Harbor Freight vibrator I have not used yet so this may be a good reason to get it set up.
What kind of Walnut shell and grit do you use and where do you get it?
Thanks for the feedback on feeds and using a 4 flute for finish passes. I have 2 flute beaten into my head for aluminum but that makes sense.
Best,
Nathan

Walnut shells will not take of machining marks unless maybe if you leave them in there for an eternity (days, if not weeks). Plastic pyramids (which must be used wet) will remove machining marks in 1-2 hours, leaving the surface looking like it was media blasted. It will also remove burrs, and put a very small radius on all the edges. You can then polish it using ceramic balls or rods with a fine abrasive (dry), and finish polish with walnut shells and rouge. But the last two polishing steps will still take a day, perhaps two. And, you can't put a lot of parts in each run, or they'll scratch each other up.

Regards,
Ray L.