PDA

View Full Version : Trouble cutting steel with TAIG



L2A3
03-10-2008, 09:05 PM
I can't seem to find the ideal speed & feed for cutting shapes thru 1.5" DOM steel tubing on my taig cnc. The wall thickness is .065 The shapes turn out smaller than than the programmrd size and usually with uneven edges. When I cut the same things in aluminum tubing- things are perfect. The bit size used is .125. I've tried 2 flute hss at 1650 and 2600 rpm at 1,3 & 5 IPM. And .125 4f carbide at 4200 and 6700 rpm 3.5, 4, 5 IPM. Things were smoother and less vibrating with carbide and the cut shapes were larger in size than with the hss bit, but the do not match the programmed size like cutting in aluminum does. Any suggestions or ideas?? I spent a good part of the day getting nowhere. Is this machine too wimpy to cut steel?
Rick

.xXACEXx.
03-10-2008, 09:30 PM
just a thought ..as i have never used a taig mill.but are you cutting one pass and in the "climb cut" if you cutters are dull and you are going around the outside in a counter clockwise manner the cutter may be pushing off "into" the part you are trying to cut if you are climb cutting,maybe your cutters are dull ,your cutting speed "looks" ok but again ive only used the big "meat eating" mills and lathes...maybe some else can help ya with more experiance on a taig... :) good luck

cjdavis618
03-10-2008, 09:39 PM
How does it sound when you are cutting? Like it is an earthquake or really whinny?

I think your RPM is to high, but I don't have a taig to compare or test with. I believe that if you run the 2 flute around 600-1200 rpm, you will be better off. But exactly what speed will be determined by the sound from the cut? ;)

Someone will be along shortly though.

L2A3
03-10-2008, 09:42 PM
I am contour cutting in 2 passes, the second being a finish pass of .05". And yes, the tool path is a ccw direction. The piece drops out after the first path and then the finishing cut occurs. I guess I have to check the shaft rotation don't remember what it is , but I don't have a choice that I know of on a taig. All bits are brand new. The hss are cheap enco, and the carbide is, well carbide. To avoid any confusion, I want the contour left in the steel tube, not the piece that drops out. It does sound like the bit is "pushing" away from the outside edge. Maybe I should reverse direction of the toolpath?

L2A3
03-10-2008, 09:50 PM
cjdavis,
the slower it goes the more rumbling & vibration. 1650 was pretty rough. Next slower is 1050. The taig has 6 speeds via step pulleys. Things were noticeably smoother at 4200 & 6700 rpm, but still not "sweet" sounding. There is a different sound between cutting along the x axis and y axis. The former sounds smoother than the latter.

Oldboy
03-10-2008, 09:56 PM
I don't have a taig? But I do have a Sherline.
Mill Steel? Stick with 4 flut cutters. Softer metals 2 flut.
Your end mill cutters will flex a little,try very very light cuts & play with your IPM. This will help keep the cutters from flexing. RPM? Try highest and work down in RPM. Cutting fluid?

L2A3
03-10-2008, 10:05 PM
I forgot to mention there is flood cooling in the set up. Since I am contour cutting along a radius, it plunges thru the tube, goes to the ist position and cuts out the pattern. Then repeats that for the finishing pass. Thanks for the 2f/4f and start high, work low suggestion. You certainly have to be methodical about this or you end up going in circles. Wish I knew that this morning

L2A3
03-11-2008, 12:14 AM
ust a thought ..as i have never used a taig mill.but are you cutting one pass and in the "climb cut" if you cutters are dull and you are going around the outside in a counter clockwise manner the cutter may be pushing off "into" the part you are trying to cut

Ace,
I went out to the shop to check the direction of motor rotation and sure enough, I have been climb or "down" milling! I'll reprogram the CAM tomorrow and have the tube feed from the other direction and hope for better results. Thanks to all!!!!!!!!!!!!

cartertool
03-11-2008, 03:28 PM
You got tons of good advice, but I would also probably only do a depth of cut of .033" and do it in two passes for your roughing cut.


The wall thickness is .065

Felipe
03-11-2008, 04:49 PM
hi!

I have a Taig and sometimes I have had the same problem. In my case I had a lot of play in the screw and in the ways. Adjusting everything solved the problem. From what you say that it sound difernet in X direction than in the Y direction its possible that you have one of the two axis with morre play than the other.

Good luck

Felipe

L2A3
03-11-2008, 05:09 PM
Nick,
I meant to say the contours run parallel and across the tube radius so selecting a varying depth of cut isn't in the cards. It has to go entirely thru the wall thickness before cutting the toolpath. At least in my CAM software it does. I can't program the bit to hug the radius as it travels along at a constantly changing z depths.

Felipe, I hope the axis' don't have too much play, the machine is very new & few hours of use, but you never know.I was thinking to check the stepper motor tuning. That in itself isn't exactly a measurable science that I know of. I ordered some TiN coated cobalt bits for "aggressive cutting which seems to be an appropriate description of what I'm doing. They can be run 10-25% faster than hss, which places their sfpm into the range of the built-in Taig speeds. Thanks for the advice. I try it again with conventional milling tonight and see what happens. After that, I'll check the ways for adjustment. Really appreciate the fast help from everybody. Great Board, great people.

L2A3
03-11-2008, 08:18 PM
Much better results. I tried it again using conventional milling and figured out how to set the CAM program to make multiple passes before going to full depth. Its .010 smaller than the plan design, which is a huge improvement but I think some additional tweeking of feeds & passes will eventually get it right.

.xXACEXx.
03-11-2008, 10:15 PM
machining is all relative..dont matter what you doing...on something you just program it to go here go there and get a good part the first time...i have been running cnc lathes for several years, and one thing i still do is "tool wear" a tool in,.. which is set the tool to cut a certian size ,then adjust it to actually cut at the size i need,by for example program a finish profile leaving .010 thousanth for a finish cut then i use the offsets to "move" the tool away exactly that much ,run the program and check the part which "should" be bigger because of moving the offset..then simply move the tool to get it to cut the right size ,this is on very heavy cast iron machines....so its all relative...im only guessing on a smaller taig machine you will have to make smaller cuts and adjust tool diameter to get the size you need.. i know this is sorta irrelavent to a mill in a way,.. but in another way its all machining. sorry for boring yall with this long post :)