Need Help!- Rapid to machine home relative

[chipsinpan]

What is the correct way to move my table to a location in reference to home relative ?
If I program a rapid move at the end of a program to change parts , and do that as a position in relation to a g54 or g55 , I risk an overtravel if I dont put the vise in the same location every time .
I know that if I write the location down as a g54 zero location ( param/coord/g54) I can do a g53 to go back there later .
Today after running into an overtravel , I just used jog to physically move the table where I wanted it to rapid to for a part change , then toggled to work3/G56 which I was not using , then set an X/Y zero . Then went back to params/coord/G56 and wrote down the X/Y values . Edit program and put these values in the last event .
Now I can be assured that this program will never run into overtravel , although it may not necessarily go to the exact location I want to change parts at . I am sure there is a better way to go about this , so tell me how !
I have tons of programs that I (incorrectly) put in rapid moves as G54/G55 positions instead of home /rel.

[pixburghenat]

Hello,

Please, correct me if I'm wrong.

But couldn't you change the G54/G55's to G53 and reference from the home position this way? I'm assuming the moves are at the end of your programs and at the tool change?


pix

[Bubba]

If I am reading you correctly, you want a point to go to at the end of the process to get the spindle out of the way to change parts etc.

What I do on my machine is set up a virtual fixture (I use G59) and when I do a tool change or part change, do a G59 G0 X0 Y0.

I do this, as I do not know until setup exactly where I will want this specific location. However, the post processor in my cam doesn't care and just puts the appropriate code in place.

Hope this helps and I have read you post correctly.

[chipsinpan]

Bubba ,
as I read it you are saying that G59 ,( which would be work 6 ) is used as a
virtual fixture , meaning a theoretical one . Then you physically move to the location you want to change parts and call this XY zero , program a position as work coord 6 /X 0 / Y 0 / G00.
I guess this is doing the same thing I explained , and as long as I never use
G59 for an actual work location , I could just leave it set , and it would get me close . I could fine tune it as needed.
I just thought there would be a more proper way to do this .

Where is JPAWELK when I need him ?

[Bubba]

Yep, you got it! This way, I don't care where G59 X0 Y0 is when I cam it, but I determine this when I do my setup. I rarely use more than a couple of fixtures so I settled on the "standard" of using G59 as my tool change/ parking position.

Also, this requires NO manual changes to my g code! I let my cam do its thing and then select my parking/ tool change position based on the setup that I have.

[cam1]

Hi:
For our VMC I modified the Post to strip out the X0 on a G28.I used to get annoyed when the table moved to X0.
e.g.
G28 Z0 ;retract Z
G28 Y0 ;push table fwd.

This pushes the table towards me (most of the time the vise is centered on the table)
Works for me.
regards

[jpawelk]

If you want the axis to move to a position relative to the machine home position, command a G53 for X and Y axis. For the Z, command a G53G49.
(Example: G53X15Y0 or G53G49Z0)