18i-T G28 on axis with absolute address only

[gregormarwick]

Is there any way to use G28 on an axis that has no relative address while explicitly omitting an intermediate point?

The sub on our Doosan is B, and only B. No way to command a relative move. So if you have a work offset applied to the B axis you must ensure that you command a safe intermediate point when using G28 to send the sub home.

Other than using G53 (which doesn't trigger the home position state), is there a "correct" way to do this with G28?

 

[hotiron]

Is there any way to use G28 on an axis that has no relative address while explicitly omitting an intermediate point?

The sub on our Doosan is B, and only B. No way to command a relative move. So if you have a work offset applied to the B axis you must ensure that you command a safe intermediate point when using G28 to send the sub home.

Other than using G53 (which doesn't trigger the home position state), is there a "correct" way to do this with G28?

I just came across this same scenario on my Mori ZL-150S. I had to forget about setting a G54 B Zero at the face of the part. I had to jog the face of the collet on the sub spindle and record that position to write into my program. Naturally G28 B0. first move was to go to the part zero first and then home. I have Fresh bar already pulled out with the sub spindle followed by a part off. I had to use all G53 to approach the part, swallow it, clamp and pull. at that point I could successfully do a G28 B0. This surfaced when turret 2 was inoperable becuase B axis didnt record a home position with G53 B0. That was my workaround anyway...code below.

N1
M100 (***************************************)
M35 (SPINDLE SYNC ON)
M101 (***************************************)
M211 (COLLET OPEN)
M102 (***************************************)
G0 G53 B-16.29 M252 (IN SPINDLE AIR BLOW ON/APPROACH PART)
G98 G1 B-17.99 F50. (SWALLOW PART)
M257 (IN SPINDLE AIR BLOW OFF)
M210 (COLLET CLOSE)
G4 U1.
M103 (***************************************)
M104 (***************************************)
G98 G1 B-15.365 F100. (PULL BAR FOR PART OFF)
M105 (***************************************)
M106 (***************************************)
M36 (SPINDLE SYNC OFF)
M05
G0 G28 B0.

 

[gregormarwick]

Thanks, I was also using a work offset to set the sub against the part zero on the main when I ran up against this.

My workaround was to use G28 B#5006 (B axis current position on my machine). It's neat and all, but I don't necessarily like it as a solution for some of the other guys who won't understand it.

 

[Ox]

My E (your B) is home at 28.7
I just code in E28.7 when I want to go home.
It doesn't fluctuate with my offsets.
Does yours?

Also 18i-T


-------------------

Think Snow Eh!
Ox

 

[gregormarwick]

My E (your B) is home at 28.7
I just code in E28.7 when I want to go home.
It doesn't fluctuate with my offsets.
Does yours?

Also 18i-T


-------------------

Think Snow Eh!
Ox

No, it doesn't fluctuate, and that would physically send it home, but it doesn't activate the homed state, which AFAICT only G28 does.

Annoying little things don't work if the B is not homed, like the tool setter.

 

[Ox]

Apparently you just got this machine?


Hey Locknut - you out there?


------------------

Think Snow Eh!
Ox

 

[gregormarwick]

Apparently you just got this machine?


Hey Locknut - you out there?


------------------

Think Snow Eh!
Ox

Nah it's not new, same one we've had for a few years now.

Just haven't come up against this before because I've always used absolute coordinates with no work offset for B before now...

 

[Vancbiker]

Switching to G code group B or C would allow you to use G90/G91 for absolute/incremental designation. Then G91 G28 B0 would be effective.

Unfortunately U and W would no longer work, you would have to use G91 for incremental X and Z moves. There are a few other differences that would additionally make switching a PITA.

 

[chucker]

I thought in G90 you could just us current position and it would work just like in G91, say your at B-10. you would put G28B-10. you are already there so it goes straight home.

 

[aj]

I was lurking, looking at your code and noticed it looks like you're transferring control from the right side to the left side to take care of opening and closing the left collet at the proper time. Have you tried controlling the left collet from the right side program with (I'm assuming) M10/M11? That way you wouldn't have to keep transferring control back and forth from the right side to the left side to open/close the left collet. For me at least, it makes things a bit easier to keep track of especially during restarts.

 

[gregormarwick]

Switching to G code group B or C would allow you to use G90/G91 for absolute/incremental designation. Then G91 G28 B0 would be effective.

Unfortunately U and W would no longer work, you would have to use G91 for incremental X and Z moves. There are a few other differences that would additionally make switching a PITA.

I think I probably have too much time invested in the post for this machine to go and switch now.

I thought in G90 you could just us current position and it would work just like in G91, say your at B-10. you would put G28B-10. you are already there so it goes straight home.

Yeah it does work like that.

In this case it was a setup for an unattended run, so I was using torque skip to failsafe various parts of the transfer. So, I didn't always know exactly where B was when I needed to call G28, hence why I ended up using G28 B#5006.