B0 programming for Multiple Offsets for a HMC and get indexes correctly.

[crazy^millman]

Hello everyone I was asked this question in a private email and thought I would share with others what I shared with them.

How do you program for P1 B0 and P2 B0 and get indexes between each face using the same tools?

Best Process is to force a tool change between the parts for those operations. Then the post will output the B0 for each face, but not between operations where it is not needed. In the Post’s understanding of what is being sent to the operations are never indexing. The machine is always kept at B0 when you make a WCS for new each part even if they are in different planes in the Mastercam file. I have found this is where the programmer needs to make groups and then control the output with force tool change when changing parts with the same tools. Now the group acts like place markers to help the programmer know where to index. I like to make Tool Number Groups. Then Sub Groups with operations 1-4 are for PART 1 P1 B0. There are in their own toolpath group for that part. Then PART 2 P2 B0 operation 5-8 are under a new Sub Group with a Force Tool Change on the 1st operation in that sub group. Now the post know that is a different part on a different face. Now if parts get moved on the machine to B90, B180, B270 no worries. On the machine that offset gets put into the offset page and controlled that way. This method means not having to worry about having the post output each index. This is beneficial in an environment where the setup may change  and parts get moved to different index positions on the machine. I have attached a link to a Mastercam 2021 files showing what I am referring to. Along with code using basic MPFAN.

Screen Shot

5TH AXIS P1 B0 P2 B0 EXAMPLE

NC Code

[Leon82]

I had a part in Camplete for the 5-axis I was trying to do this and I had the same problem when I was at a0c0 it wouldn't index with the new work offset. I ended up running all three programs in succession.

 

43 minutes ago, lamlapphuong said:

hi! i use post mp master 4 axis i usually output coordinate G54-G59 when rotary axis and now. i want to output coordinate work TCPC . only G54 can you help me! please thank you

You have to set all your planes to zero for the work offset

[Colin Gilchrist]

3 hours ago, Leon82 said:

I had a part in Camplete for the 5-axis I was trying to do this and I had the same problem when I was at a0c0 it wouldn't index with the new work offset. I ended up running all three programs in succession.

 

You have to set all your planes to zero for the work offset

There is a setting in CAMplete to make the software treat each new Work Offset Number as a separate "index". I'll see if I can take a screenshot when I'm back in the office. I'm training a customer on a new OKK VC-X500 today.

[cncappsjames]

This setting will allow you to have multiple part coordinate zeros in a single setup.