CAMPLETE TruePath and Force Tool Change

[Bottlecap19]

Wondering if anyone has had any experience with this? When using the same tool for a different operation, Force Tool Change throws in a pull up, M01 and all that jazz; however, when using CAMPLETE as the post processor it seems to ignore this completely. Any way to force it to stop between operations with the same tool?

 

Thank you.

[nickbe10]

6 minutes ago, Bottlecap19 said:

Any way to force it to stop between operations with the same tool?

Have you tried the Camplete Forum?

[Guest]

You could add a manual entry between the operation with an m00 inside, but don't forget to to add the mcode to start the spindle after. For example m00 then s10000 m03 or whatever spindle speed you need. 

[Guest]

the spindle speed declaration should be on the next line btw

[Guest]

its possible you could renumber your tool and assign multiple tool numbers to the same pocket but keep in mind that means multiple tool offsets as well.

[Leon82]

I did it

I have a post somewhere here about it

You need two format macros.

One in the 3+2 transition block and another at the top of the 3+2 start block

The start block needs basically the tool change.

 

The transition macro needs to cancel the two, tool change, reinitialize twp.

 

[Leon82]

Also there is a setting you have to check to recognize the force tool change in one of the settings pages

[Leon82]

So the top two boxes are slightly incorrect. I can copy the correct macro calls.

 

[Leon82]

On 5/10/2019 at 4:49 PM, nickbe10 said:

Have you tried the Camplete Forum?

Do you have a link for the complete forum? It doesn't shot up in Google for me

[tim_h]

When I post through CAMplete for our 5 axis it doesn't recognize Manual Entry or Force Tool Change... sadly

Maybe its in the settings ??

[Leon82]

2 hours ago, tim_h said:

When I post through CAMplete for our 5 axis it doesn't recognize Manual Entry or Force Tool Change... sadly

Maybe its in the settings ??

Yes go into options and I believe it's file types.

It will say mastercam on top and scroll through all those settings in the bottom of the window.

 

There should be one that says set nci force tool change operation parameter

[tim_h]

thanks Leon82 

I'll look into it when I get a chance.

[Leon82]

I can't type too much now but you may get error saying that there's a missing parameter.

 

if you look in the thread link I posted earlier in this thread you'll see set ignore missing parameters on you're going to need to add that line to your macro call 

[Leon82]

Ok,

 

So I. Assuming you have a 5 ax machine and are using the 3+2transition block.

You need to make 2 macros. You can call them anything but make it so you know what they are doing.

One will be force change same orientation

The other will be force change different orientation.

At the start of the 3+2block you have to call the different orientation maco with the clause if prev tool =current

 

At the start of the 3+2 transition block you need to call the same orientation macro with the clause if prev tool=current.

 

The different orientation macro needs just the tool change and mo1 basically.

 

The same orientation macro need alot more. It will basically need to cancel twp, m01 and re initialize the twp.

If you do not use the built in codes and initializations it will not be simulated. Custom gcodes are not simulated. G53moves are simulated 

There are macro call in the thread I posted . That datum clause won't do what I originally thought so it's should not be in there.

[crazy^millman]

There is a process in CAMPLETE to control all of this and they handle all of this very nicely one you have defined the process in your control setting for the machine. Get a hold of their tech team and they will walk you through what is needed and how to accomplish this task.

[Leon82]

Is that  a new feature?

We had them look at ours and they did not mention that.

[Leon82]

If you edit the machine using  the secret button combo you can edit the tool changer cycle and tool break cycle

 

You can upload all the control macro variables and the fanuc parameter file.

You can make custom parameters also but you still need to tell it what to do when it sees the parameter