High Feed Machining - Is it possible to vary spindle speed in operation as well?

[Ryan Green MLC CAD Systems Inc.]

I've just started experimenting with using High Feed. I've got the perfect job for it now, so I've got a good reason to finally get into this. I have figured how to setup the parameters, from material setup on through the tool feed parameters. I've got a part that is profiled on the table which is now standing vertically in a vise. I am surfacing an irregular blade edge onto one side of the part, using a 5/8 iscar multi-master ballnose tool. I have an STL of the part before this op, using it to drive the high feed parameters. It will post the variations in feed just fine.

 

My question is this: Is it possible to make the spindle speed vary throughout the cut as well, depending on what edge of the ball profile of the tool that is in the cut?

[Matthew Hajicek - Singularity]

I don't think so, but it would be a good feature request. Send it to support(at)mastercam.com

[Watcher]

Nope.

 

I believe that CNC software would have to redesign the entire High-feed coding, what I think it´s not in their plans at all...

 

But Vericut does it. One more reason why I think they would not have any interest on this matter...

 

But I´m not CNC software spokesperson, so maybe I´m hugely wrong.

 

Sorry for my hopeless feedback.

 

JM2C

[Ryan Green MLC CAD Systems Inc.]

That's cool. I figured that if it wasn't an obvious parameter, it must not be an available feature. Maybe in the future!

[Jon Griffin CNC Software]

DMG Austin,

 

Spindle speed doesn't vary in highfeed, but please send in the request to support. It's the best way to see about getting your feature into the product.

[Ryan Green MLC CAD Systems Inc.]

I actually already did that, and I got a reply back saying they thought it was a great idea. I guess we'll know, in time, if it was a good one...

[mold100]

The first company to land this will set there place forever, this has been a constant chip load issue for alot of years, could you imagine a spindle varying spped and acurite with the feed rate, it would be sick, how many cutters could handle it if it were not perfectly in sync.

 

Toolpath goes from 80 to 400 ipm, alot faster than the spindle could go from 3800 rpms to 9800.

 

It will be a bigger task for machine tool builder than software development IMO.You have to add a dwell for certain machines to adjust spindle speeds thus de utilizing the high feed path.

[andrewgore]

I asked about this before even in non high feed machining. Plunge rate and feed rate need different spindle RPM's if their feed rates are different. I've usually just ended up editing the gcode when I need to do this. Course, people thought I was crazy when I brought this up. lol. Maybe I am, but then again, I don't think a sparkingchattering tool is crazy; Nice light show yes....fun,...no.

 

Andrew

 

ps, I will send another request to qc. I might have just brought it up with my reseller in the past. Can't remember

[Matthew Hajicek - Singularity]

If you wanted to get fancy you could write it into your post. Maybe have a Misc. Real for the ratio of RPM to IPM, and recalculate RPM whenever IPM changes.

[Darren Long SPE]

I think Heidenhein iTNC530 has a constant chipload option in it.......

[mold100]

Again my question is how many people believe the spindle can accel and decel at the same speed the feed rate changes, I for one do not think any machine tool could go from 200 sfm to 1000 sfm, if you watch the control over something complex programmed at 400 ipm the feedrate may drop all the 60ipm, then boom back to 2 or 300 ipm, the spindle can not do that IMO, most spindles take a few milliseconds to reach 15,000 rpms and to go from 15,000 to 9500 to 15,000 It can not keep in sync with the feedrate (If this what this thred is all about) just my .02

[Guest CNC Apps Guy 1]

If you've got a direct drive spindle, you prolly need 1/2 sec to go from 3800 to say 10,000. Geared spindle... fuggeddaboudit! 1-2 sec MINIMUM, then on top of that, say you dwell... in some nice work hardening material... that'll leave a mark

 

I do think it's s great idea though... ONLY in certain machines, certain materials, and certain conditions.

[Greg_J]

quote:

---

I think Heidenhein iTNC530 has a constant chipload option in it.......

---

Feed rate in MM per spindle revolution:

M136?

 

This is what the Heidenhain book says about it:

"With M136, the TNC does not move the tool in MM/Min, but rather at the programmed feed rate in MM/spindle revolution. If you change the spindle speed by using the the spindle override, the TNC changes the feed rate accordingly."

 

M137 cancels M136

 

Would that work in the reverse? Use Highfeed Machining and it has all the feed rate changes in the program and that would adjust the RPM?

 

Greg