Tool returns home after each operation

[cadscout]

We are using Mastercam v9. The problem one of our operators is having is that after every operation (drilling, contouring, etc.) the tool returns home as if for a tool change when there is no need for a tool change. It appears to be a configuration issue, but I can't find the area to change the default.

 

Can anyone give me any ideas on where to look and what to change.

 

Thanks, Tony

[Odin]

Is block skip turned off on the machine? ours was doing that and we turned block skip on.... it doesnt return to home position after every op now.

[Bryan Johnson]

check the setting for "Force tool change" on the toolpath parameters.

[bogusmill]

Force tool change will do what you describe

[PeterM]

V9 had no "force toolchange"

I'm thinking that its in your post, mpmaster posts behave that way when going from one named view to another.

[DavidB]

quote:

---

V9 had no "force toolchange"

---

Not True

 

 

I do believe it is a post issue though.

Are you using the MPmaster?

[Jim Evans from CNC Software]

Is there toolchange calls in the NC or is the machine doing this on it's own?

[Superman]

Have you rechecked your WCS & planes ?

 

Have you programmed in TOP for a horzontal and then trying to machine at other planes thet may not be quite correct ?

 

I've had a similar problem where tool retacts after each op. on an incorrect set-up (plane)

 

Verticals -WCS=TOP T/plane=TOP, FRONT, BACK etc

Horizontals-WCS=TOP T/plane=FRONT, LEFT, RIGHT etc

[Colin Gilchrist]

Good man Dave, you saved me the trouble...

 

Cadscout,

 

You should also check and see how you are handling setting the part coordinate system. Check the header of your PST file. Does it have this:

 

code:

---

# mi1 - Work coordinate system 

# 0 = Reference return is generated and G92 with the

# X, Y and Z home positions at file head.

# 1 = Reference return is generated and G92 with the

# X, Y and Z home positions at each tool.

# 2 = WCS of G54, G55.... based on Mastercam settings.

---

You might just have MI#1 set to "1" and the post is generating a home position move at the end of each tool...

 

How do you normally set your work coordinates? G54 or do you use G92???

 

HTH,