Zero Return

[Phil Orenstein]

The ususal zero return at the end of program I'm familiar with is thusly:

G91G0G28Z0.

G28X0.Y0.

 

However I just got one I've never seen:

G53X20.Y0.Z0.

This was generated from a MPYang.pst post.

 

Does anyone else use this type of zero return? What the difference? Just curious.

Phil

[Guest CNC Apps Guy 1]

G53 is Fanuc Machine Coordinate System, must be specified in absolute mode (G90) and is a one shot code.

[chris m]

As usual James is correct. The only real differences, I think, are that you don't need the G91 / G90 with G53 that you do with G28 and that I don't believe you can specify an incremental clearance move with G53 like you can with G28. We use G28 in our Fanucs [habit] but I use G53 in our Haas because that is their recommendation.

 

C

[Guest]

And interestingly enough...We have some Matsuuras that need a G53 Z0 or tool changer no workie

Jim

[connormac]

The only thing you have to worry about in moving all 3 axis at one time is if anything is in the way you could crash.

[Phil Orenstein]

Again, as always I am humbled by the wealth of knowlege amassed here. Yes, I agree the similtanoeas movement has to be changed. If I break it up into 2 lines and put the Z0. first so it homes in Z, do I need the G53 on both lines as with the G28? In other words, is the G53 modal or non? What should I add to the Yang post to accomplish this. I'll be able to get to the post on Mon when I'm back in the office.

 

Thanks,

Phil

[connormac]

I'm a chicken. To be on the safe side I would put G53 on both lines. I don't know about your machine but on my machine if I don't tell exactly where to go sometimes it seems to try to go to the break room or smoking area before hitting limit switches.

[tryon]

G53 is non-modal. one shot on the line its on.

[Thad]

I'm with tryon...non modal.

 

Thad

[George_Gerhard]

As many people have already said G53 is the machine coordinate system, there must be a G53 on each line, and this must be done in absolute. A command of G90 G53 X20. would send the x axis 20 inches or mm from the machines home. G28 on the other hand works in G91 (incremental)it can work in conjuction with the plc the signal is zpx, zpy, zpz, the plc can use this for many reasons. Some manufacturers use G28 to turn on reference return led's on the operators panel. Where G53 would not typically do this.

 

rgds

George

[Phil Orenstein]

Thanks for the explanations, but I still don't quite understand the need for incremental G91's on the G28 line. It seems redundant - the G28 can stands alone as a zero return, I think. Anyway, I like to understand what's the reasoning behind the code.

 

Any takers on my other question - how to modify the post for 2 separate G53 lines?

 

Phil

[connormac]

Need to see your post. peof# section. Shoule be able to help.

 

Kyle

[George_Gerhard]

Phil

If you use G28 with G90 the machine will move to the programmed zero point then go home

 

rgds

George

[Phil Orenstein]

Thanks. Here's the peof section:

 

quote:

---

peof0 #End of file for tool zero

peof

pbld, n, "G53", "X20.0", "Y0.0", "Z0.0", e

 

peof #End of file for non-zero tool

pretract

comment

#Remove pound character to output first tool with staged tools

#if stagetool = one, pbld, n, *first_tool, e

pbld, n, "G53", "X20.0", "Y0.0", "Z0.0", e

n, "M30", e

"%", e

---

[Allan]

code:

---

peof0 #End of file for tool zero

 

peof

pbld, n, "G53", "X20.0", "Y0.0", "Z0.0", e

 

peof #End of file for non-zero tool

pretract

comment

#Remove pound character to output first tool with staged tools

#if stagetool = one, pbld, n, *first_tool, e

pbld, n, "G53", "X20.0", "Y0.0", "Z0.0", e

n, "M30", e

"%", e

---

Change that to this:

code:

---

peof0 #End of file for tool zero

 

peof

pbld, n, "G53", "X20.0", "Y0.0", "Z0.0", e

 

peof #End of file for non-zero tool

pretract

comment

#Remove pound character to output first tool with staged tools

#if stagetool = one, pbld, n, *first_tool, e

pbld, n, "G53", "Z0.0", e

pbld, n, "G53", "X20.0", "Y0.0", e

n, "M30", e

---

That will split up your moves

 

Allan

[McRae]

G28 is the return to home "Thru a Point".

 

If you specify an axis move of G91 Z0. - then an incremental move of "Zero" Inches/MM in the Z Direction will take place before the machine goes to the reference position. You could use G28 in Absolute and specify a height to retract to above the part ie G90 G28 Z10. This would be usefull for a retract move on a horizontal before you swing the pallet and the G29 will bring you back thru an intermediate point as well.

 

Hope this clears up the reason for the Incremental Switch.

[Phil Orenstein]

Allan - Thanks very much for that!

 

Phil