On my taig, if I'm milling a circle and it is not coming out perfectly round, what could I be doing wrong? I'm milling bearing seats and doing both roughing using conventional and finishing using climb cutting (climb is only taking about 8 thou off).
Any tips on where to start looking for the prob?
I'm using the 280oz steppers and a xylotex drive. I've generated the G code using RAMS for the circles.
Thoughts or hints would be appreciated...
check your backlash
1-Check ur backlash
2-check that the setting for x-axis and y-axis leadscrew mapping is correct in controller software(Mach3 etc)
How is it not round? Is it ovaled? Or are there little notches at certian positions, etc?
For critical applications you should not make bearing seats this way. Bore it on your mill or turn it on a lathe, never profile mill it (if it's critical).
It will never be perfectly round if you profile mill it. How much out of round is it.
Regards
Phil
.Originally Posted by b0gh0s
It depends where it is out of round and by how much.
Errors at the direction change points (12, 3, 6, 9 o'clock) are typically caused by backlash and take up errors in your drive'ball screws.
Out of roundness at 45 degrees off the vertical or horzonal axis are due to servo tuning errors. At this point, both servor are affecting a high rate or change in opposite directions. Unless the tuning is perfrect, you;ll start getting follower error and out of roundness.
Don't think for a minute that "backlash comp" will "fix" backlash problems - it won't. SOftware can NOT predict or compensate for uncontrolled/uncontrollable motion that occurs due to slop. You may not have a "perfect" machine which may be why you have some out of roundness. However, EVERY effort made to eliminate slop/backlash/etc or hother forms of lost/unpredictable motion will result in improved cuts and predictable geometries.
BTW, if you spend the time and money, you CAN tet mills to mill ROUND holes to amazing levels. However, it takes time and care and some5times more money than its worth, especially on a ''hobby" lathe/ or mill.
You could also use a rotary table to profile a bearing seat with an endmill.
Phil
Thanks for the responses guys,
The holes are coming out out of round at about a 45 degree oval to the table
Assuming this is a tuning issue, any thoughts on how to go about fine tuning the stepper setup in Mach 3? I know how to change the settings but what should I look for in fine tuning?
I'm assuming this means i need to fine tune the # of steps/inch metric in the motor tuning area? Any references from other taig owners with a xylotex, 270oz stepper and Mach 3 setup?
re-reading the posts, I'll go back and tune up for backlash. Still confused on how to tune the steppers to help correct this though,
Check your gib plates, most likely you're dealing with missed steps like I was.
How deep are your passes ?
What's your feedrate ?
Sounds like a backlash issue, once you measure and input backlash into Mach it should come out round within a half thou or so. You will never get a perfectly round hole by this method though, it's always be off a bit.
In motor tuning all should be 32000 steps/inch with Xylotex.
Also make sure the head is trammed square in both x and y...
Nick Carter
Largest resource on the web about Taig lathes and mills
www.cartertools.com
Thanks guys will do. I'm assuming something got moved/loosened in my recent move, but I'll go through it with a fine tooth comb.
I'm cutting plain old 6061 with 5/32 2 flute carbide for the roughing, (taking 6hundreths each pass in depth) and running at around 2500rpm. Doing my finishing passes at full depth taking about 8 thou of material off in climb cut with a 4 flute 5/32 carbide EM.
Mill does not sound like it is chattering or loading up really bad and I'm using flood coolant.
Posting Permissions
LinkBack URL
About LinkBacks
