visualmill post for cent6 vm15

I need a little help figuring out an issue I have with the post for my vm15 cent 6 :o
1) for every tool change I cant get the tool # offsets to post . If I understand this right , you need this (G43H0 D01)for the tool change with a tool changer ? :o

T5M06
S6000M03M08
G43H0 D01

2) At the end of the program the head crashes to the table . I'm thinking it has to do with the G00Z00 in this part . What I have been doing is , erasing this end lines and inserting a tool change to stop it from crashing . It works , but is there something I should change in the post processor ? same with the tool offsets .

G40G49M09
G00Z00
G00X0Y0
M05M30
END
%%

I'm kinda learning the hard way :o but getting there ,I think :o

Steve

Steve,

You need your tool offset call to have a corresponding offset number, not just H0, so your G43 line should look like this:

T05M06
S6000M03M08
G43 H05 D05

Now, you don't always have to have the offset and diameter numbers be the exact same as the tool number, there are cases where you might use two different offsets on the same tool, but.... in general, you always number the D and H values the same as the tool number.

Once that specific tool offset is active, then at the end of each tool, and at the end of the program, you put in a G40G49Z0M09 line.

Make sure that you put the offset # into the callout during your tool creation.
IDK your control but you may need a G53 or G28 in your end code.
The post processor is 100% customizable in VM

Quote:

---

Originally Posted by Brian L

Steve,

You need your tool offset call to have a corresponding offset number, not just H0, so your G43 line should look like this:

T05M06
S6000M03M08
G43 H05 D05

Now, you don't always have to have the offset and diameter numbers be the exact same as the tool number, there are cases where you might use two different offsets on the same tool, but.... in general, you always number the D and H values the same as the tool number.

Once that specific tool offset is active, then at the end of each tool, and at the end of the program, you put in a G40G49Z0M09 line.

---

thanks Brian , I've been editing the G43 line after I post . The end of program was the main concern

Quote:

---

Originally Posted by DareBee

Make sure that you put the offset # into the callout during your tool creation.
IDK your control but you may need a G53 or G28 in your end code.
The post processor is 100% customizable in VM

---

How do you change the tool change in the post processer ? I can see where to change the end of program .

Steve

Change it in the tool change tab

I would expect the last line of your first load tool macro to look like this
[SEQ_PRECHAR][SEQNUM]Z[NEXT_NONMDL_Z]H[TOOL_ADJST_REG]
this line does NOT include D offset and you would have to add it as well with the [TOOL_ADJST_REG] behind it.

You may need to play with the other tool change macro as well.
My machine holds the [TOOL_ADJST_REG] as modal for subsequent changes