O-ring inproving marks left by entry exit and surface finish

B

Bob Gray

Plastic

Joined

Nov 13, 2007

Location

Redwood City

• Mar 10, 2021

• #1

Hi, see attached pictures. The part is made from 304 stainless steel. As you can see from the attached pictures I'm getting marks on entry and exit. The application is vacuum and I'd like to get the surface finish so I do not have to spend time on secondary finishing if that is possible. Different brand of end mill, more time in the machine etc is not a problem.

Right now I'm running an Imco M9 series 1/8th end mill 4 flute. I use a slotting operation to remove the bulk of the material leaving .005 on the floor for cleanup. The I use a 2D contour to to cut the sides to finish dimension. I've tried a Harvey tool 1/8th with corner radius but get a similar result. Then a finish for the floor to minimize cutter deflection. Speed-feed plus chip load is in the pictures with plunge etc..

Thanks

 

TrollTuner

Aluminum

Joined

Jul 11, 2015

Location

SW Missouri

• Mar 10, 2021

• #2

Ramp entry should help. I have had good luck with the Garr VRX Through collet coolant helps too..

 

S

Slugo

Aluminum

Joined

Feb 24, 2007

Location

Connecticut

• Mar 10, 2021

• #3

Leave .01-.015 on the floor for finishing not .005 Also are you using a rougher and a finisher or just one tool as your surface finish is not that great anywhere.

 

0

007Rob

Aluminum

Joined

Sep 24, 2015

• Mar 10, 2021

• #4

Can you finish the wall and the floor in seperate operations?

Ie. when you finish the floor stay a .001" or so away from the walls and then when you finish the wall stay up .001"

 

B

Booze Daily

Titanium

Joined

Sep 18, 2015

Location

Ohio

• Mar 10, 2021

• #5

Can't read your speeds and feeds, but that finish looks terrible. What machine are you running this on?

 

B

Bob Gray

Plastic

Joined

Nov 13, 2007

Location

Redwood City

• Mar 10, 2021

• #6

Only using one end mill for both rough and finish. I'll order the Garr tool and use the Imco as a rougher. Try leaving more for finish.

 

dandrummerman21

Stainless

Joined

Feb 5, 2008

Location

MI, USA

• Mar 10, 2021

• #7

What kind of machine are you even running?

 

Hardplates

Stainless

Joined

May 8, 2019

Location

What once was a free country

• Mar 10, 2021

• #8

If the code looks good, doesn't plunge Z past the floor, it looks indicative of shitty servo tuning or mechanical backlash on a machine with a counterbalance.

As was already asked, what machine?

If it is a machine issue that doesn't mean you can't work around it with careful programing such as slow smooth moves and a vertical arc in, as was already mentioned.

 

dandrummerman21

Stainless

Joined

Feb 5, 2008

Location

MI, USA

• Mar 10, 2021

• #9

I had missed that someone already asked what machine it was on.

But I imagine all these suggestions on fixing the issue, all to find out that's it a little homebrew cnc.

Like hardplates said, you can probably work around it even if it was. probably. But if it really is critical vacuum stuff, I'd think you'd be needing to lap it anyway? (never done that kind of work myself.)

 

B

Bob Gray

Plastic

Joined

Nov 13, 2007

Location

Redwood City

• Mar 10, 2021

• #10

Haas VF-2. I zoomed in with a microscope. So to the naked eye the finish looks passable. But under a loop 5x you can see the tool marks.

 

Hardplates

Stainless

Joined

May 8, 2019

Location

What once was a free country

• Mar 10, 2021

• #11

As I said you need to check the code. If that is good then I would check for backlash in Z. A vertical ramp will likely hide some short comings if it is machine related.

I know nothing about Haas machines and if it is a option but bell shaped accel deccel curves will help with overshoot when plunging at a high feed rate.

I have loose machines and tight machines. I can make good parts on them all, it just requires a different approach and amount of time.

 

B

Bob Gray

Plastic

Joined

Nov 13, 2007

Location

Redwood City

• Mar 10, 2021

• #12

I'll play with Fusion and see what Lean in lead outs are available...

 

Rick Finsta

Stainless

Joined

Sep 27, 2017

• Mar 11, 2021

• #13

I can't read any of that toolpath information, but use a 2D contour and not a slotting operation for this. That was you can use the "ramp" option on the linking tab and ramp down. That's how I cut o-ring grooves and I have never had a problem with finish.

ETA: also, get rid of your lead out or you'll usually get a toolpath that gouges since it isn't processing the model geometry, just your selected contour.

 

Last edited: Mar 11, 2021

E

evega

Plastic

Joined

Jul 22, 2018

• May 20, 2021

• #14

For the dwell mark, I'd start by a slower feed in the Z move once the tool is +.02 from the floor. End mill tips are the high point of the tool so slow it down or just ramp in. I'd definitely over lap the start and exit point to make sure that area is covered again.
As for the rest of the o-ring surface tool marks, try pushing the feed rate up. Milling is funny like that, a harder feed can polish and can even help remove the step during face milling.

 

C

codeine01

Plastic

Joined

Sep 24, 2018

• May 20, 2021

• #15

The lead-in lead-out parameters are on the last tab in the edit 2D contour tool path in Fusion 360. You can remove any lateral lead in/out and use a small purely vertical lead-in/out at 90 degrees with perhaps a 0.020 to 0.050” radius. This eliminates abrupt axis motion stopping and machine directional change that can result in a small vibration, not enough to cause a dimensional change (per se) but a small cosmetic change ( the swirl marks you see here).