[colton_m]

Hey guys,

I have a quick question regarding (what I would hope to be) a simple post edit for MCX2.

I am programming a hitachi seiki mill with a Yasnac control using the generic 3axis vmc post that came with X2.

I have edited most of the post already to include simple things like zeros in all the g-code e.x. (G02 instead of G2) so far everything works great.

However,

When I call up a tool (M06) I am curious as to how I can have Mastercam look ahead and queue up the tool for the next operation? (My will has an external 30 pocket tool changer). It's a heck of a lot faster if the tool carousel does it's huge rotation while the previous operation is underway... Instead of starting to turn when the next M06 command comes up.

It's simple enough to add in manually after the fact but it becomes kind of a pain when the program has more than 10 tool changes!

Thanks,
Colton.

[Superman]

In the machine definition file under "Tools", place a check of "Pre-Stage tools".

If it still is not pre-staging, then it would also need enabling in the post
search for "stagetool" , I would say it is currently set to zero or n/no
stagetool : 1 # 0 = no, 1 = yes

[colton_m]

In the machine definition file under "Tools", place a check of "Pre-Stage tools".

If it still is not pre-staging, then it would also need enabling in the post
search for "stagetool" , I would say it is currently set to zero or n/no
stagetool : 1 # 0 = no, 1 = yes

Awesome, it's running smoothly now.

For anyone curious it was set to "0" (options being 1 or 0)

Thanks,
Colton

[Xavior]

Sent a PM to Superman about this, but in the mean time i figured id post about it too.

I tried to follow your instructions but im finding its not working in the program. I even went ahead and tried to edit the post to get it to work but no go.

I have mastercam x5, here is my post:

stagetool : 1 #SET_BY_CD 0 = Do not pre-stage tools, 1 = Stage tools
stagetltype : 1 #0 = Do not stage 1st tool
#1 = Stage 1st tool at last tool change
#2 = Stage 1st tool at end of file (peof)

In mastercam x5 machine definition manager, under tool changer group, right click on automatic tool changer and hit properties.

From there i selected "No indexing/pre-stage tool" under indexing method.

The post spits out a program like this:

N120 T1 M6
N130 G0 G90 G54 X6.563 Y0. C0. S1528 M3
N140 G43 H1 Z2.
N150 M88
N160 G98 G81 Z-1.35 R-.1 F4.6
N170 X15.188
N180 X23.813
N190 X32.438
N200 G80
N210 M09
N220 M5
N230 G91 G28 Z0.
N240 G28 Y0. C0.
N250 M01
N260 T3 M6

As you can see it does not call the tool up before the machining. Any ideas?

[Superman]

In mastercam x5 machine definition manager, under tool changer group, right click on automatic tool changer and hit properties.

From there i selected "No indexing/pre-stage tool" under indexing method.

As you can see it does not call the tool up before the machining. Any ideas?

Your problem is this bit, you've changed the machine def layout... instead of the actual Control Definition file ( in your post it says "SET_BY_CD"....meaning that file actually switches it )

Re-reading my last post, it should have said
--open the MMD file, then access the associated CD file, then go to the "Tools" tab