surface finish

[ligrow]

I am using MCX on an assortment of CNC mills. Roku-Roku, Fidia, Sharnoa, Fadal, Brothers. I used to get pretty good surface finishes but lately my programs have been getting choppy. I get swirl marks and cusps in my finish no matter how small the pickover. Actually the smaller the pick the more the program seems to stall. I have tried mastercams filter but this only seems to make things worse. Is there any way to tweak the machines or mastercam to achieve better finishes. Custom post are an option but a very exspensive one.

[Carl Hessig]

What's your spindle speed. If you have a high speed spindle and your using collet chucks the collets could be worn out and might need to be replaced. Drop one on the floor it may look ok but finish will start to suffer.

 

Carl

[ligrow]

No Sir,

 

No collet chucks here, using Tecnara heat shrink tooling. I understand that cutter length, size, ect. can effect the finish. What I am getting is a jerky toolpath. It almost seems like the look-ahead in the machines will not work together with the filtering of the programs in mastercam. If I turn the filter off completly the program will run smooth but my finish suffers.

[Guest]

What are you running for feedrates?

[Jeff2005]

This is easily taken care of with your total tolerance setting (cut tolerance). I run mine tight and I get a better finish.

[ligrow]

I usually run everything at 200ipm and the spindle will vary with the cutter, usually around 7500 rpm or faster. We are an edm shop and cnc cut our electrodes out of graphite. As I said in the earlier message if I use the filter settings (total tolerance settings) it actually seems to make it worse. I have noticed this since we went to MCam 9.1 and then on X bigtime.

[Guest]

I would try slowing the feedrate down and see if that helps.

 

Roughing at 200 IPM is one thing, I know my Mori's do not like finishing at 200 IPM on any kind of XYZ surfacing. I run them at 135 IPM or so and they seem to do OK.

 

 

JMO

[gavetta]

I'm not sure about some of the other machines, but the Fadal has a code that "ramps"down feeds at the end of every linear move as to reduce over run. Check your Fadal manual for details. I think it's something like a G98 maybe but not sure on that.

[crazy^millman]

G8 for the Fadal and do you notice this problem on every machine when you post the code or just one particalar machine. I would also compare code on a part. I would do the same toolpath, filter settings and everything in V9 and X and compare the code. If you see a big difference then I would start to question the post and what are your tolerance setting for the post in the CD. If you have a Nc verfiy like Predator, Metal Cut, or any other look at the path created by both and compare you should see it there as well if you do then Zip everything up shoot it to [email protected] and your dealer and see if it is a possible bug.

 

HTH

[ligrow]

All my machines have the look-ahead feature on them. They automatically slow down in corners and for ramping on surfaces.

[Shawn Wentzel- Wenteq Inc]

I have a 1998 haas that does the same thing. I turn the filter on and set the total tol on the parameter page (not the filter settings page) to around .00004. This solved my problems but still I couldn't go that fast. I have a new haas though that i can put a filter on at .001 and run around 600-700 IPM finishing with no problems.

[Chris Rizzo]

quote:

---

I have a new haas though that i can put a filter on at .001 and run around 600-700 IPM finishing with no problems.

---

600 ipm on a haas? our new one at 150 ipm for surface finishing is about all she'll take. ...although your filter is pretty loose.

[kinglouie V]

I like the G08

 

 

quote:

---

(FINISH BOSS)

G0 X-1.9726 Y-.5868

G08 P1

G1 Z-.059 F10.

G41 D1 X-1.7226 F4.

G3 X-1.4726 Y-.3368 I0. J.25

G2 X-.6774 I.3976 J0.

X-1.4726 I-.3976 J0.

X-1.4601 Y-.2379 I.3976 J0.

G3 X-1.6401 Y.0665 I-.2422 J.0622

G1 G40 X-1.8822 Y.1287

G08 P0

G0 Z.1

M05

M9

---