1. Home
  2. ⋐⋒⋐ Computer Numeric Control
  3. Holding a tenth all day on a high speed mill!

Holding a tenth all day on a high speed mill!

First of all, if you have no laser for tool pickup...move on. Read about the arab crap instead.

Setup...2 fanuc makinos, 10 yrs old. Both have new spindles, and one has new leadscrews. machines run 24/7. Even holidays. You will have to adapt this stuff to your setup obviously, but its universal if you figure out how to do it on each brand.

This is a thread to throw some tips out there, if you disagree tell us why, if you cant...again...go read arab posts.

First 4 tips! I have a bunch of em!

#1) First...add an orientation code to the tool change macro. What this does is assure that every tool is picked up the same by the spindle, helping repeatabilit. Make sure and orientate when getting a tool and when putting it back. You want the same conditions every time.

#2) Add a 30 second dwell to every finish tool to stabalize the spindle!..

#3) Try to group tools by rpm. Try to not have a big spead in rpm from one tool to the other.

#4) Clean the spindle every setup.Clean every toolholder with a ruby stone, keep the tools as short as possible. And make sure everything is balanced, be anal about it. If you cut off a cutter with a cutoff wheel, grind the end, it makes that' much of a difference.

#5) Use the laser inteligently. Do not do it manually one at a time. Make a program, set eah cutter to laser at the rpm its programmed at. Add a 120 second dwell to first tool, and a 60 second dwell to all others. If you have to laser a single tool, make sure you laser them ALL again. It must be done all together to get a perfect spread. Keep people away from the machine when it's lasering.

6.)on a comparitor, map out bull cutter readii, measure the diameters, etc...its called mapping out the cutters. Input this into your cad proggy.

7.) be sure your spindle oil is full if it cools the spindle. The more there is the better the core temp will hold. (hint...fanucs for the most part run the chiller when the spindle is turned, even if just bumped by hand. So turn the spindle by hand it chill.)

8.) feedrates! Do a cut, watch the feed, if its slowing down in corners its feeding too fast. What you want is a steady feed. Corner control is great, variable feedrates SUCK. Learn how it can take a corner,, and program feedrates as needed. Remember, the rpm is not sycronised with the feed, So if ts slowing down in corners, its not adjusting rpm...this just eats cutters like nothing else.

9) Holders. .0002 runout is the max. The coating is only a tenth deep, so if you run out 3 tenths, it strips that flute of its coating, then wears like crazy. if your using collets and think they are good enough...exit out of your newsreader.

10) timing is everything. You cant run non stop....go to lunch, and think it will be the same. It wont. try to pace yourself, same time between loads etc...

11) I got a bunch more...stay tuned for part 2.

Reply to
vinny
Loading thread data ...

If you program IPR instead of IPM the feed and rpm are synchronised.

Reply to
Alphonso

on a mill?

And if yes, can the spindle changes keep up with the feed changes? Because this is the dream of all high speed millers, syncronised speeds and feeds with corner control. Wow that would be awesome.

Reply to
vinny

Yes,on a mill. With IPR the FPT is synched to the spindle. I don't see why you couldn't change the feed on corners or arcs and then go back to original feed on straights.

I have a Reed Prentis WWII vintage mill that has the feeds in IPR. The first time I ran a CNC mill I couldn't figure out why my feeds were all so slow until I realized that the mill was in IPM.

Reply to
Alphonso

Iv'e tried this on a haas, and the spindle couldnt change fast enough. The machine jerked out from it. Maybe on a higher end machine it could work ok?

Reply to
vinny

In IPR mode, does the control take into account the rad of the tool? I use IPR for 5 axis machining, never seen how it works on profiling.

I do not see any need to change spindle speed, cutting speed must be kept c onstant. Load per tooth must be kept constant too, and feedrates must chang e for internal and external rads, but it depends on the rad of the tool.

I don't think the usual Fanuc controls can do it, and even if some do I wou ld not use it, move the job to dumb one and the problem comes back. And one day an operator will forget to input the tool diameter into the control so I prefer the feedrates changed by CAM software.

Esprit gives you variable feedrates for corners, is one of the good points of this POS, together with cutting speed and load per tooth.

DanP

Reply to
DanP

In IPR mode, does the control take into account the rad of the tool? I use IPR for 5 axis machining, never seen how it works on profiling.

I do not see any need to change spindle speed, cutting speed must be kept constant. Load per tooth must be kept constant too, and feedrates must change for internal and external rads, but it depends on the rad of the tool.

I don't think the usual Fanuc controls can do it, and even if some do I would not use it, move the job to dumb one and the problem comes back. And one day an operator will forget to input the tool diameter into the control so I prefer the feedrates changed by CAM software.

Esprit gives you variable feedrates for corners, is one of the good points of this POS, together with cutting speed and load per tooth.

DanP

************** Mastercam 9 came with a chook proggy that was just what your talking about. You could tell the software to slow down on corners with a certain angle or a certain gforce. It worked way better than fanuc corner control because you could tweak it over time for a particular machine. However, you still couldnt control the rpm, and not that it mattered, the machine could not speed up or especially slow down fast enough to matter.

The option now is at the machine, turn down the feed/rpm until corner control is bearly changing the feedrates.

Reply to
vinny

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.