Post outputs M3 but not M4

[Randy Morton @ Clem Industrial]

Is there any logic to why this would be? What should I check to fix this up?

[Guest]

try using a minus speed -4500 see if that does it

[Randy Morton @ Clem Industrial]

You cannot put a minus in the speed box...

[Guest]

Lathe or Mill,

 

I just did it in mill

 

code:

---

G00 G90 G54 X-.2 Y-.06 S6500 M04

G43 H2 Z2. M08

G98 G83 Z-.2788 R.1 Q.03 F30.

G80

X-.926

G98 G83 Z-.2788 R.1 Q.03 F30.

---

[Randy Morton @ Clem Industrial]

Sorry, Lathe. =]

[calnet42]

Try this:

Define Tool from tool manager or from operation

Select "Setup Tool"

Change Spindle Rotation

[Randy Morton @ Clem Industrial]

Actually, all my tools are custom defined to run in M4, and I have been using them for a while now with great success.

 

This morning I just started hacking away at the MPFan.pst file, trying to get it up to snuff the way I want and noticed it only does M3's, but no M4's. So, I know it's not the custom tooling direction.

[Randy Morton @ Clem Industrial]

Alright, who moved my post??

[Guest]

I did,

 

Not really an off-topic, seems very much on topic for the main forum

[Randy Morton @ Clem Industrial]

I know. I posted in the OT by accident.

 

Any other thoughts on the 'topic' at hand then?

[Jamie Betz from InterTech Supplies]

I run into problems like that when I setup a tool to run CCW in the tool setup and then when you pick the tool to use in an operation it makes the spindle speed a negative number and will only post a M3, but if you remove the negative sign in front of the spindle speed then it will post the M4. It is almost like the negative spindle speed is canceling out the CCW spindle direction in the tool setup, this is in router but it seems like it might be just mastercam in general. I have mentioned this before but it doesn't seem like anything has ever been done about it.

[Randy Morton @ Clem Industrial]

I sent my stuff off the Brett @ In House and he helped me out. Maybe this can help you too, Jamie. Works like never before now...

 

code:

---

pcss            #Output Constant surface speed

speed = g_speed

if css_actv$,

[

if css_start_rpm, pbld, n$, *sg9697, *speed, pspindle_l, !css_actv$, e$

else, pbld, n$, *sg9697, *speed, pfspindle_l, !css_actv$, e$ #Force if not called after G97

]

!speed

---

I replaced my pcss with this and it worked fine. The explanation he gave was that the spindle was not stopped priorly and thus you need to force the rotation.

 

Makes sense, but it still seems weird that I was getting like 3 ops good and 4 with no spindle, even with an M1 or M00 in there.... ahh well. Works great now!

[Jamie Betz from InterTech Supplies]

Awesome, I will give that a try and see if it works for me to. Thanks Randy and Brett.