Post Edit Help

[Gecko]

I would like to edit our mpmaster post to return the table to front and center at the end of the program to make life a little easier for the machinist. Post editing is very new to me and my boss doesn't like me experimenting with his equipment

Can i do this with a g28 or g53?

thanks

[Jimmy Wakeford from Barefoot CNC]

If it is a fanuc control you can use the G53 and give it a "machine" x/y coordinate to go to.

G91G28 can alo be used, but I think a G28 will cause it to go home 1st then to the coordinate.

 

YOu could type in the line on the floor to test it.

[Gecko]

Jim

Thanks, i am currently adding code to the end of the program manually. I'd like the post to do it automatically to prevent any errors. I am unsure how to modify the post so it will output the neccesay code.

[Clarence]

Someone suggested a while back to use an unused machine offset. I have several Haas machines with different X travels so I use G110 and set that in my offset page. Therefore I don't need to make a specific post just to center the machine.

[3rdstring]

Look for the peof$ section of your post & add the desired code in that postblock.

 

HTH

[Colin Gilchrist]

Make the following changes to the peof$ (end of file post block)

 

Original:

 

code:

---

peof$            #End of file for non-zero tool           

pretract

if lock_codes = one & rot_on_x, pbld, n$, *sunlock, sunlockcomm, e$

rotretflg = 1

pbld, n$, *sg28, "X0.", "Y0.", protretinc, e$

rotretflg = 0

if lock_codes = one & rot_on_x, pbld, n$, *slock, slockcomm, e$

comment$

if not(index), n$, *sg90, e$

n$, "M30", e$

mergesub$

clearsub$

mergeaux$

clearaux$

"%", e$

---

Make the following changes:

 

Change the {*sg28} to "G53" if you want G53 instead of G28. Then change the {"X0."} to "X20." or whatever X value you want. Same for the Y value. The code below is for G53 X25. Y0. output.

 

code:

---

peof$            #End of file for non-zero tool           

pretract

if lock_codes = one & rot_on_x, pbld, n$, *sunlock, sunlockcomm, e$

rotretflg = 1

pbld, n$, "G53", "X25.", "Y0.", protretinc, e$

rotretflg = 0

if lock_codes = one & rot_on_x, pbld, n$, *slock, slockcomm, e$

comment$

if not(index), n$, *sg90, e$

n$, "M30", e$

mergesub$

clearsub$

mergeaux$

clearaux$

"%", e$

---

[Gecko]

Thanks alot guys

[heeler]

You could also use a manual entry toolpath at the end of your program. This will allow you to put different values for different machines.

 

Glenn

[Colin Gilchrist]

Shouldn't you have different posts for different machines? Besides, if you add the manual entry, you would also need to delete the G28 home moves, as the peof$ post block is called after all toolpaths (including manual entry) are finished...

[Guest]

I personally like using a misc real to import a value of my choosing.

 

Gives more more flexibility and I am not locked into 1 table position

[Colin Gilchrist]

Thats what I ususally do on my posts too John.

[bigjohn]

Don't forget to make a copy or two of the post before you do any alterations.

 

 

John