Roughing and Finshing Passes

cmmpro1 · Jan 4, 2018

Good afternoon everyone,
I am working on a project and it seems to be taking too long to run. When milling, I take a roughing pass leaving about .005. Then I take a finishing pass. Is it that needed? I want to make sure the part looks good and not leave tooling marks. Thank you in advance for any help on this.

DMF_TomB · Jan 4, 2018

cmmpro1 said:
Good afternoon everyone,
I am working on a project and it seems to be taking too long to run. When milling, I take a roughing pass leaving about .005. Then I take a finishing pass. Is it that needed? I want to make sure the part looks good and not leave tooling marks. Thank you in advance for any help on this.

.
depends on how much cutting forces roughing passes were taking
.
normally leave .003 to .030" for finish passes. i have often seen where .020" was not enough to clean the rough milling chatter or vibration marks
.
facemill going over 50 ipm feed can put 1000's of lbs of force on a part
.
sometimes rougher leaves .030
semi finish pass leaves .003
that way finish cutter taking a relatively light cut

michiganbuck · Jan 4, 2018

You might look at cutter lines on the part.. With a feed of .020 per spindle revolution and one line every .020 then only one flute is end cutting. You might set opposite inserts to the same height ..If an end mill do a better job of sharpening..If the mill is out of tram perhaps only one side of the cutter is in play. Might use an end cutter with more flutes and yes precision sharpened.
A custom sharpening with having perhaps .015 flat at end would/may make a better surface finish.

You might just cut down your rough feed rate to rough and finish in one pass if that works..and saves some time...?

Some times a heavy cut will stress the cutter enough to make it one side end cutting or even vibrate the part, and then the light cut allows the cutter to cut flat and the machine smooth so cutting both sides for better finish.

triumph406 · Jan 4, 2018

cmmpro1 said:
Good afternoon everyone,
I am working on a project and it seems to be taking too long to run. When milling, I take a roughing pass leaving about .005. Then I take a finishing pass. Is it that needed? I want to make sure the part looks good and not leave tooling marks. Thank you in advance for any help on this.

That's pretty much what I do, leave .005 (or so) and then a finish pass. If I'm feeling generous I might take 2 finish passes, especially if size is important

Finegrain · Jan 4, 2018

How much is being taken of during roughing? What material? What feed and speed during roughing?

It's hard to get a fabulous finish and rough in the same toolpath. Cutter is a lot more engaged during roughing so the chips are more likely to get recut, or the tool is flexing, or the work is flexing, or the material is tearing a bit, etc.

Also hard to HSM and finish at the same time. HSM is fast and furious, but not generally lovely.

Regards.

Mike

DMF_TomB · Jan 4, 2018

roughers are made for heavier cuts at higher ipt feed. 55 ipm feed is normal as long as 1 ton part not vibrating so much you can easily hear it over 100 feet away and leaves chatter marks over .020" deep
.
those same inserts make a poor finish
.
modern finisher inserts you can usually see reflection in finish. not saying you can read a tape measure but definitely can see its a tape measure

michiganbuck · Jan 4, 2018

Good finegrain mentioned chips.. sometimes if chips are breaking a coolant or air shot can get chip to be less a problem.

DMF_TomB · Jan 4, 2018

horizontal cnc often has fire hose like blast of coolant coming from ceiling to blast chips off part and pallet table and force them down to chip conveyor.
.
forget to turn on chip conveyor it plugs with chips and over flows and a big puddle of coolant around the cnc from overflow

DavidScott · Jan 4, 2018

What works best for you with your needs on your machine is up to you and it takes time to figure out. You failed to say what materials you are working with. For me, in aluminum, I often leave .001" or nothing for the finish pass. Even with a stiff box way machine there is always metal removed when I rough to net then finish. Tools used for finish do matter. Some tools leave a better finish than others at high feedrates, I have yet to find a better one than Destiny Tool, their 3 flute mill is almost as good as the Harvey 5 fluters in aluminum.

DMF_TomB · Jan 4, 2018

DavidScott said:
What works best for you with your needs on your machine is up to you and it takes time to figure out. You failed to say what materials you are working with. For me, in aluminum, I often leave .001" or nothing for the finish pass. Even with a stiff box way machine there is always metal removed when I rough to net then finish. Tools used for finish do matter. Some tools leave a better finish than others at high feedrates, I have yet to find a better one than Destiny Tool, their 3 flute mill is almost as good as the Harvey 5 fluters in aluminum.

even aluminum bigger parts when heavy roughing have vibration chatter marks many
rougher leaves .020 to .030
semi finish leaves .001 to .003
that way finish cutter uses very little cutting pressure deflecting part
.
another reason is after roughing when vise or clamps released part distorts or bends. rechucking to machine this distortion out often requires extra cuts. i have seen many parts warped .001 to over 0.100" when unchucked

cmmpro1 · Jan 4, 2018

michiganbuck said:
You might look at cutter lines on the part.. With a feed of .020 per spindle revolution and one line every .020 then only one flute is end cutting. You might set opposite inserts to the same height ..If an end mill do a better job of sharpening..If the mill is out of tram perhaps only one side of the cutter is in play. Might use an end cutter with more flutes and yes precision sharpened.
A custom sharpening with having perhaps .015 flat at end would/may make a better surface finish.

You might just cut down your rough feed rate to rough and finish in one pass if that works..and saves some time...?

Some times a heavy cut will stress the cutter enough to make it one side end cutting or even vibrate the part, and then the light cut allows the cutter to cut flat and the machine smooth so cutting both sides for better finish.

I saw that option while I was setting up the program. I am sort of new to CAM. Does that work in the same fashion as making two separate passes? (Roughing Finishing pass)

michiganbuck · Jan 4, 2018

If you mean cutting down the feed rate..That may or may or may not work. Add up the total time doing it in two passes.
Then select a one pass that is perhaps 1 1/2 that time (just selecting a slower feed rate for the rough pass)...Just try the same rough-cut amount and see if the finish is good enough..
That way you still have the stock on the part to finish if needed..and only have to finish off with using the same program as used before...

This way you preserve the original program so it is easy to go back to two passes.
What material and cutter? look at the cutter and see if it seems all teeth are cutting the same..If an indexable cutter you can indicate the inserts and see that a few are the same height at the end cutting.

cmmpro1 · Jan 4, 2018

michiganbuck said:
If you mean cutting down the feed rate..That may or may or may not work. Add up the total time doing it in two passes.
Then select a one pass that is perhaps 1 1/2 that time (just selecting a slower feed rate for the rough pass)...Just try the same rough-cut amount and see if the finish is good enough..
That way you still have the stock on the part to finish if needed..and only have to finish off with using the same program as used before...

This way you preserve the original program so it is easy to go back to two passes.
What material and cutter?

Thanks for the info. I am cutting aluminum using a 3inch shell mill and .375 4 flute for the contour.

michiganbuck · Jan 4, 2018

You might run the shell mill by hand backwards to indicate the outer down tips to see that the cutter runs .001/.003 or so close to being all the same height..I know you cant do much because it is a solid cutter, likely a tight ft to spindle and the face quality of your spindle nose..

.003 is a lot IMHO

Search

Largest Manufacturing Technology Community on the Web

Search

Roughing and Finshing Passes

cmmpro1

Plastic

DMF_TomB

Diamond

michiganbuck

Diamond

triumph406

Diamond

Finegrain

Diamond

DMF_TomB

Diamond

Attachments

michiganbuck

Diamond

DMF_TomB

Diamond

DavidScott

Diamond

DMF_TomB

Diamond

cmmpro1

Plastic

michiganbuck

Diamond

cmmpro1

Plastic

michiganbuck

Diamond

Similar threads