About machines with corner control...

You are correct. It does sux and it is being addressed. Technologies such as HSM, Hardmilling and Micromilling can greatly benefit by this.

Software has tried to work this out but the problem is that getting the unique machine dynamics into software is quite an effort. It never gets it right. Software doesn't know my machines all that well so it's a rather complex issue.

The good th> There's machines that lower the feed as needed to hold a location within a

But crank the average high speed mill up a few grand, it takes like a few seconds and eats up the load on the spindle. As the spindle speeds up horsepower is lost for that moment, creating another condition of unequal cutting feeds and speeds. Slowing down might be acheivable? Thats just a breaking action.

Damn it would be cool to hear a mill wind up and down as it mills. Hell that would even sound efficient as hell.

The key is to use a toolpath that doesn't make sharp corners, so the machine doesn't *have* to slow down. I would tell you to just use the Dynamic Mill toolpath, but NX doesn't have it, or anything comparable.....

As a test for your machines, in NX program a contour using SFM instead of rpm. Select corner control and cut the feed down say 40% in the corner at 50% of tool (just enough to make a difference). I know on a very old Mazak 5ax it worked well. That said the machine had some balls to its spindle. We mostly programmed SFM so if the operator used the feed override, the chip load remained the same.

-- Bill

e:

A little birdie told me.

Same reason Surfcam calls it "TrueMill", Celeretive calls it "Volumill", and Cimco calls it "Adaptive Clearing." It sounds cool.

Because that's not what I want.

Jon

I don't think you understand vinny's statement. He is speaking about servo control. Controlling machine dynamic motion vs actual commanded (nc code) motion during the reversals. It's a rather common practice on high end machines during HSM and HD milling with real time servo control. It has a large impact on part quality in regards to accuracy, cycle time and surface finish. Anytime you have a change in direction in motion (ex. block to block) you have an angle of change (free form machining). The steepness of that angle will be calculated and the control will slow down to hold a desired corner tolerance and then speed back up. When the machine slows down, your chip load changes and there becomes the problem. In most cases it's not huge problem but can be a major problem in micro machining when chip loads change. Cut with a .002-.005 diameter end mill in harden CPM. Then it can be a problem in this case.

The only way to truly hold accuracy during HSM is to have the control handle servo lag. Your CAD/CAM can not do this?

These are all toolpath engagement solutions. This will soon be at the control. We can check for real time spindle loads monitoring torque and all aspect of the spindle. The key is to make on the fly adjustments during the entire machining cycle.

Now imagine if you could place a sensor along the length of the cutter to monitor deflection, internal heat while encompassing that with the information feedback from the spindle.

As a test for your machines, in NX program a contour using SFM instead of rpm. Select corner control and cut the feed down say 40% in the corner at 50% of tool (just enough to make a difference). I know on a very old Mazak 5ax it worked well. That said the machine had some balls to its spindle. We mostly programmed SFM so if the operator used the feed override, the chip load remained the same.

-- Bill

so your saying... Program the machine with a constant feed to rpm ratio, adding a slowdown in the corners so it will output different rpm's going in and coming out of corners, to see if the machine can change rpm fast enough.

That would at least prove if the machine can do it from the program. If it can than there's no reason the manufacturer can't add that into HSMilling to do it on it's own.

good idea.

If I get access to any of the machines in the near future I will post my results.

Yes.

No (imho). Reason being there are many variables to when and what distance you may want to tool to slow down. If you look in NX you'll see you can set the angle by which it decides it's a corner. Then you can set the distance from the apex that the tool starts slowing. Also you can create several steps along the way to slow down. It was one of the refreshing things to see having had to use MCX for a short time. They had a similar function for this but it was an all or none high speed milling operation module as I recall.

-- Bill

Bot sure about x, but mastercam 9 had a thing somebody donated, started out as a chook, then they stuck it on the ops page. It was feed control. Damn it was awesome. You could actually give it a gforce and save it with a name of a machine. then after time you could tweak in your individual machines by just bumping that number up or down. Plus it had variable ramp up or down on the feed. I havnt used it on UG yet, just looked at it. looks almost the same. I bet if I look hard enough it will do all those things.