Forcing a D2 at every Cutter Comp in post

[Frank]

Hi All: We just got our new Makino A81 delivered. I'm trying to get the post edited to work right with this machine. It sounds strange but the nc file must only use H1's (tool offset) and D2's(cutter comp)for every tool in the rack. It actually sounds pretty scary, is anyone familiar with this ? I was able to change the post to only use H1's but I can't find where I have to change the D's to only use D2, can somebody help.

 

Thanks,

Frank

[Guest CNC Apps Guy 1]

Sounds like Tool Life Management. Not scary at all.

 

In your Post, do a search for "G43" and replace "*tlngno" with "H1" and repeat until they are all changed. Could be on there as many as 3-4 times or more.

 

Next do a search for the "pccdia" post block, find "tloffno" and replace it with "D2".

 

Thst should do it if memory serves.

 

As always, make a back up of your post, and if you are unsure about what to do, seek the services of a qualified professional who works with posts for a living, (i.e. your reseller, etc...)

 

HTH

[Mike Whitten CAD/CAM Contractors]

Frank,

 

I have run many Makinos in the past and IMO, this is a much better and safer way.

 

Anyhow, I went back and checked my old tool library and here is what I did. I just put H1 and D2 on the Tool and have Job setup set to "from tool" The advantage of this vs hard coding it is that on special close tol jobs, you can overide the D# to something else. You may want to hard code the H though.(I would)

 

Although I did not do it back then, I would set the post up so that there is safetys(prompts when posting) that warns you if the H value is not 1 and the D value is not 2

 

HTH,

Mike

[specv]

code:

---

 pccdia          #Cutter Compensation

tloffno = 2 ##added tloffn = 2

#Force Dxx#

if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno = c9k

sccomp

if cc_pos, tloffno

---

This is what i did so it forces a D2 everytime.

[Frank]

Thanks all: James I always ask my reseller, but this sounded like an easy fix for the great minds here. I would of had to send my Mc9 file, my post, and txt file, and my generated nc file without edits, then one with. Also normally their backed up so it would of taken a month to get it back. I'm sure there is more to change, but I wont know until I get more familiar with the machine. This was a quick fix, with a quick question. Thank you it works great.

 

Frank

[Guest CNC Apps Guy 1]

So is your machine using Tool Life Management?

 

The only thing that makes putting it in the Tool Parameter pages tough is it forces you to remember to put those values in when you create a tool. Too much for me to remember personally, that's why I prefer to deal with it in the post. If you wanted flexibility, you could always create a Misc. Int, that you couls use to define a tool as using Tool Life Management which would then force a H1 and D2 otherwise, it would be as normal.

 

 

James teh limitless possibilities...

[Frank]

The machine has tool life management, but I'm not real familiar with it, and the great minds here don't want to use the free schooling to learn it. How's the learning curve ?

 

Thanks,

Frank

[Guest CNC Apps Guy 1]

Well, with the amount of talent in here, the learning curve is pretty much nil. You basically have to register tools in groups like so...

 

code:

---

O11(TOOL LF MGMT REG - JAMES MEYETTE)

( )

(LAST EDIT: XXXX - XX - XXXX- JRM)

( )

(USE THIS PROGRAM TO REGISTER TOOLS INTO -)

(TOOL LIFE MANAGEMENT. YOU CAN SPECIFY -)

(FREQUENCY TYPE BY PUTTING IN A Q VALUE -)

(BY OMITTING A Q VALUE, CONTROL WILL-)

(DEFER TO PARAMETER #6800.7)

(MACHINE HAS 128 GROUPS)

(TWO TOOLS PER GROUP MAX)

(P = GROUP NUMBER)

(L = TIMES OF USE BEFORE TOOL EXPIRATION)

 

 

G10 L3

P1 L9999 Q1 (GROUP 1 - 9999X USE - TYPE FREQUENCY)

T1001 H1 D201 (2" FACE MILL - ALUMINUM)

 

 

P2 L9999 Q1 (GROUP 2 - 9999X USE - TYPE FREQUENCY)

T1002 H2 D202 (2.5 FACE MILL - STAINLESS STEEL)

 

 

P3 L9999 Q1 (GROUP 3 - 9999X USE - TYPE FREQUENCY)

T1003 H3 D203 (.750 VARIMILL CHAMFER- STAINLESS STEEL)

T1003 H4 D204 (.750 VARIMILL CHAMFER- STAINLESS STEEL)

 

P4 L9999 Q1 (GROUP 4 - 9999X USE - TYPE FREQUENCY)

T1005 H5 D205 (.750 VARIMILL SHARP- STAINLESS STEEL)

 

 

P128 L9999 Q1 (GROUP 128 - 9999X USE - TYPE FREQUENCY)

T1128 H49 D249 (4.000 CAST IRON FACE MILL)

 

 

G11

M30

---

So instead of calling tool 1, you woudl call 1001 (in the case of the machines at one of my customers)

 

HTH

[Frank]

Wow it looks foreign to me. Is that above an actual program ? See if I get this right. The tool management is for automatically changing tools after one has hit a defined number of cycles, or parts. Then the next tool does the same and it picks the original back up.....

Thanks

[Mike Whitten CAD/CAM Contractors]

The Makino's I have ran all had Fanuc 16 Pro 3's and the nc program did not have to be altered. The control kept track of the tools by using FTN's (functional tool numbers) and ITN's (Individual tool numbers)

 

We have other machines here that work like the way James was saying.

 

Regardless of how your machine works, it may be fairly easy to just check it out in the manual.

 

Mike

[Frank]

We also have the pro 3. And it was explained to us that we could use just the fanuc part of the control, to use the regular offsets, but would lose a lot of the pro 3 features, like defining heavy tools in the rack, so the machine will automatically slow down the tool change, for one instance. What concerns me with this machine always using H1's and D2's is I can't transfer any programs from our Hitachi Seki to the Makino without redoing the whole program.

[Mike Whitten CAD/CAM Contractors]

Frank,

 

All you should have to do is re-post with the correct post or do a find and replace in an editor. Use an editor that has a wild character or whatever you call it. Like Find H* and replace H1.

 

IMO,

I would not even consider to not use the Makino stuff, It is very nice and easy.

 

Mike

[specv]

Frank,

We use both sides of the control, let me know what you need

[Frank]

I really don't want to have to repost this program, it's been running a couple of years, and changes don't go thru me. I'll have to use the editor to get it right. The other problem will be that the Makino doesn't take the G95 for tapping, which I thought was a great feature on the Hitachi, so that will also have to be changed.

 

Thanks,

Frank

[Guest CNC Apps Guy 1]

My bad, I used the wrong one. Here is an actual snippet of code from the TLM I registered this morning.

 

code:

---

%

O11(TOOL LF MGMT REG - VIKING PROD)

( )

(LAST EDIT: MARCH 2, 2005 )

( )

(USE THIS PROGRAM TO REGISTER TOOLS INTO -)

(TOOL LIFE MANAGEMENT. YOU CAN SPECIFY -)

(FREQUENCY TYPE BY PUTTING IN A Q VALUE -)

(BY OMITTING A Q VALUE, CONTROL WILL-)

(DEFER TO PARAMETER #6800.7)

(MACHINE HAS 128 GROUPS)

(TWO TOOLS PER GROUP MAX)

 

G10 L3

P1 L9999 Q1 (GROUP 1)

T1 H1 D201 (2" FACE MILL - ALUMINUM)

P2 L9999 Q1 (GROUP 2)

T2 H2 D202 (2.5 FACE MILL - STAINLESS STEEL)

P3 L9999 Q1 (GROUP 3)

T3 H3 D203 (5/64 CARBIDE 4 FLUTE END GARR MILL)

P4 L9999 Q1 (GROUP 4)

T4 H4 D204 (3/64 CARBIDE 4 FLUTE END GARR MILL)

P5 L9999 Q1 (GROUP 5)

T6 H6 D206 (.750 SHARP - ALUMINUM)

P6 L9999 Q1 (GROUP 6)

T7 H7 D207 (.500 VARIMILL CHAMFER - STAINLESS)

P7 L9999 Q1 (GROUP 7)

T8 H8 D208 (.500 VARIMILL SHARP - STAINLESS)

P8 L9999 Q1 (GROUP 8)

T9 H9 D209 (.375 VARIMILL CHAMFER - STAINLESS )

P9 L9999 Q1 (GROUP 9)

T10 H10 D210 (.250 CHAMFER MILL 90 DEG - 3 FLUTE )

P10 L9999 Q1 (GROUP 10)

T11 H11 D211 (.500 SPOT DRILL)

G11

M30

%

---

Yes it works as you stated except that it will not return to the other tool in the group unless you reset the number of uses the tool has acumulated. So change the tool, reset the number of cycles or seconds and you're good to go with the new tool. I woudl not consider using anything but, even if I did not have redundant tools in the magazine, it still is a GREAT feature.

 

HTH