Lathe post help - M3

[4xxx4]

I'm setting up our lathe seats for MCX2 and could use a bit of help getting it to post an "M3" or "M4" every time it posts a spindle command. I"m editing the MPLFAN for a HAAS SL-30 chucker (fanuc series 10) which is used in a perpetual state of "test drive" and it's getting pretty deep for me. I run almost exclusively prototype work and if the control doesn't see an m3 or 4 I get a "spindle not turning" alarm which keeps me adding the code manually.

How can I force it to post the spindle direction every time it posts a speed command?

 

All help greatly appreciated!!!!

[3rdstring]

look for spindl_l & change it to *spindle_l

 

HTH

[4xxx4]

Sorry Chuck but that isn't it. I did a search and didn't find "spindl_l"

 

Anyone else with a bit of help?

[Jim Evans from CNC Software]

See if you have the cool_w_spd variabl;e in your post.

 

code:

---

 cool_w_spd  : 1      #Output coolant with spindle code, 0=no, 1=yes 

---

If this is in your post and set to 1 as above, then the Coolant and Spindle commands come out as one (M13/M14).

 

Set this to zero and you will get seprate M codes for each (M3 M8)

 

If this doesn't work, then I suggest forwarding your post and MCX file to your reseller for support.

[4xxx4]

Thanx Jim but the setting you are refering to is already been set to "0" and it posts an m3 or 4 when it starts the program as well as when it drills. The problem is with CSS and subsequent tools going the same direction. I tried blocking the save spindle direction but this didn't work either. I tried inserting the spindle_l in the CSS spindle start section but I might have placed it incorrectly to get the desired results - tried forcing it as well but it seems to ignore the command if the previous tool ran the same direction.

Last time I asked my local reseller to help me customize the post, it didn't come back with many of the changes I asked for but I might see if he has any advice for this problem.

 

Anyone else?

[Jim Evans from CNC Software]

are you getting M5's in the program?

 

Was this ever working? Did someone makes mods and now it is not?

 

 

Was the MPLFAN post being used from X2 or a prior version brough up?

 

Should be something real simple. I've ran some tests with MPLFAN in X2 and it seems to be working fine.

 

Can you try one of the other LAthe MD's like the lathe 2 axis slkant bed.LMD which will use a different post and see if you get the same results and let me know what you find.

[monty]

QUOTE

-------------------------------------------

Sorry Chuck but that isn't it. I did a search and didn't find "spindl_l"

--------------------------------------------

Hi

It must be "spindle_l" not "spindl_l".

Change it to "*spindle_l", It is in pcss section.

It worked for me.

HTH

 

Monty

[4xxx4]

Hi Jim. Yes I have done extensive mods to this post. I killed the M5 because I don't want it stopping the spindle at the end of every tool. Maybe this is something that can be fixed in a next version. The stock post should only post an M5 if the spindle direction changes. It would be nice if the post would drop the spindle speed during the rapid exit move if the spindle direction changes rather than an M5. The distance to a safe index point can be taken advantage of to slow the spindle reducing cycle time for a direction change.

 

I'm trying to make it post a structure like my hand writen programming so that scrolling through the program is as short as possible. Extra pages of minutia cost me time when a problem arrises.

 

Thanx Monty!!! This worked nice. I was wondering if he typo'ed......

 

The next thing I need to do is put the tool call on the same line as the spindle command and I'm done. This might take me a while......

 

Thanx everyone !!!!!!!!!!!!!!!!!!!!!!!

[3rdstring]

quote:

---

I was wondering if he typo'ed......

---

OOOOOOOPPPPSSS!!

[4xxx4]

The odd thing to me is that I could swear I tried Monty's method.......

 

No harm, no foul Chuck. Thanx for the try