tuning the highfeed option

[peon]

I'm starting to play around with the highfeed optimization. I made a test cut with a 1/2" flat endmill, machining a 2" circle, .625" deep, 1640 rpm @ 17.1 ipm. I cranked the feed at the controller as high as it would allow which resulted in 105 ipm. There was no gouging. I plugged 105 ipm in the corner acceleration tab and which resulted in 0.007934 G's. No complaints here so far. I finally applied the highfeed option to some toolpaths (see 11588_SLIDE_FACE.Z2G on the ftp server, operations 4 and 5)which resulted in a very poor finish on the straight walls, but the corners looked great. If I turn the highfeed option off, I get the finish I desire. Anyone have any ideas on this little dillema. Thanks!

[3R!< W3NG3R]

HIgh feed for roughing and no highfeed for the finish pass?

[peon]

Both toolpaths are programmed with 2-roughing passes at .002" and 2-finishing passes at .000". The first roughing pass leaves an adequate finish, but the finish passes have scallops. Both cutters are new carbide with a tin coating which always resulted in a great finish without the highfeed. I'm assuming the feedrate is too high after the highfeed option. I have the optimization set to roughing and finishing.

[Rick Henrickson The Boeing Co.]

I have never used the highfeed options in mastercam but I would think there is parameters that need to be set to match your machine capabilties on many aspects, acc, dec, loop back time, ball pitch, I dont know but I would think these would have to be accurate.

[peon]

Hello Rick, I considered those settings, but I only have the problem on the straight areas on the perimeter of my part. The corners look nice. I think the highfeed option is suppose slow down in the corners and maintain the correct chipload according to the axial and radial depth of cuts. It appears it is handling the corners fine, but EXCEEDING the chipload in the straights.

[Rick Henrickson The Boeing Co.]

what feed is it telling it to go in the straights?

maybe it has something to do with rigidity?

spindle/ holder / tool combo

[Craig Madsen from CM3D]

You can limit the maximum feedrate in the parameters -

 

Highfeed does NOT take into account, or change, the RPM of your tool, only the volume of material removed per minute.

 

Restrict the maximum feedrate to one that is appropriate to your tools/rpm. Then Highfeed will take care of the rest.

[YoDoug®]

Highfeed works with volume removal not chipload. That is why on the perimeters its going too fast. It is trying to match the volume removal rate in the corners and straights to be the same.

[peon]

Thank you! I totally misunderstood chipload vs volume removal when using this feature. I'll set the max feedrate to a reasonable rate. Rick, the 1/2" endmill's feedrate was increased from 17 ipm to 105 ipm on the straights leaving large scallops. Thanks again folks!

[Rick Henrickson The Boeing Co.]

that doesn't seem that far out what RPM

we ran 1/2 em 3flute at 12000 rpm and 108 ipm

[peon]

The tool was only programmed at 1640 rpm @17.1 ipm (215 sfm @ .0026" chipload). I suppose I could try 1000 sfm at .0026" chipload = 7640 rpm @ 80 ipm for our 4-flute cutter. We're in a transition period and just getting into high speed machining and hard milling vs the old conventional milling. I purchased both of Dale Mickelson's books and finally starting to apply these newer methods of machining.

[peon]

Hmmm. Something still isn't working correctly. I entered a max feedrate of 55 ipm in the material removal rate tab and it still outputs over 100 ipm.

[Mark H]

quote:

---

... I purchased both of Dale Mickelson's books and finally starting to apply these newer methods of machining.

---

What did you think of his books? Are they worth getting?

[peon]

Very well worth the $$$. Very easy to read! Must have books in my opinion.

[peon]

I changed the max air cutting rate to equal the max feed rate and I think I finally got what I want.

[midnite]

Sorry..i'm beginner here

 

so.....is that mean there is no setting that we can take it as reference & then fine tune? E.g..Volume/ min=...?

 

We have to test every single tool dia & machine? Anyone has it?

[Mark Baker CNC Software]

There is a bug with High Feed (depending on the toolpath type) where the air cut parameter is switched with the max feedrate. Try switching these settings and the toolpath should work correctly.

 

I believe that the surface toolpaths are working correctly with High Feed.

[GVM]

Mattstang70, I have Dale Mickelson's first book. Is the second or newer book just a rehash? Is it worth spending 40.00 dollars if you already have the first book? Your opinion would be appreciated. Sorry for the hijack.

[Chris Rizzo]

I used to use Highfeed pretty extensively... my trick was use it only for roughing toolpaths, and always create a seperate non-highfeed contour pass after it. that way you don't have to compromise the roughing and aircutting feedrates just to deal with the finish passes.

[peon]

One book is all about modern tooling, cutters, holders, etc. The other book is all about the high speed machines like roku, johnsford, okuma, etc. It is WELL worth the extra $$$ for the second book. They go together.