I recently tried to use a G95 (feed/rev) mode on the Tormach 1100MX for a tapping cycle, but the result was the Tormach moving at a feed rate of 1mm/min.
This works well with rigid tapping for an M6x1 tap since the feed rate matches the spindle speed and the tap is 1mm pitch.
G21
G94
S1035 M03 M08
G84 G98 X132.5 Y55.125 Z-8.2 R15.5 F1035
but when using G95 i get a great way to drill with a tap. It simply seems to ignore the G95 and sets the machine RPM to 1035 and the feed rate to 1mm/min just as it would in G94.
G21
G95
S1035 M03 M08
G84 G98 X132.5 Y55.125 Z-8.2 R15.5 F1
from Tormach’s website: TAPPING CYCLE (G84) (tormach.com) i can see that it says not to use G95 for threading, not sure if that includes tapping, but i thought the entire purpose of G95 was for tapping? Does anyone know what i’m missing if G95 is supposed to work correctly? or can anyone confirm that it’s not working?
@JT_Murnyack - great question!
G95 F/rev is more common in turning than in milling. I’ve never heard of using G95 in a tapping cycle although I admit I understand the appeal of not having to do the math to calculate the correct Z feed rate.
For any less-experienced users reading this the math isn’t too bad - it’s just the thread lead times the spindle RPM.
Example for a 1/4-20 thread at 600RPM:
1/20in * 600rpm = 30 ipm.
Regardless, the behavior you describe (a 1mm feed rate) is a bug. We should either allow tapping in G95 or throw an error when a user attempts it. Thank you for reporting this one!
@JT_Murnyack I wanted to follow up with you on this issue. After researching the RS274 standard, we didn’t find evidence that G95 should be allowed during a tapping cycle. The changes required to enable G95 during tapping are challenging. Most other control manufactures don’t allow it and I couldn’t find one that specifically does allow it. We changed PathPilot’s G84 tapping cycle so that it will let the user know if G95 is enabled and throw an error. This code change should be included in the upcoming 2.10 or 2.11 release.
Thank you very much for reporting this! I appreciate your help with improving our software for all users.
G95 can have very positive attribute for milling. Although it is most often found in turning. For milling it can prevent a spindle stall. Great for noobs to machining. If the spindle slows the feed reduces. Where the machine bottoms out is where your at max performance for that cutter. Reduce rpm by 10% and fine tune with feed adjustment. Reallybgreat for low hp machines.