Doosan Large Tool

[JeremyV]

So we have a Doosan Mynx 7500...

 

My issue with the machine is this:  When calling up a large tool and then tool changing to something else.... the machine first indexes to the tool that was called up, but when the machine realizes it isn't the correct pocket, it indexes back to the pocket where the large tool is stored at then tool changes and indexes to the right tool then tool changes.  I hate that, the previous Mazak we had did not do this, the HAAS we have does not do this, our machine vendor wasn't much help, So i wondered if anyone here has a fix for it?

 

At the moment, the only thing i can think of is editing the post file somewhat so it doesn't index when "T35" is in spindle and once T35 is finished, machine tool changes to previous tool then moves onto the next tool. I don't know, maybe that's over complicating things in terms of post file...

 

So, as a result, i've been trying to avoid using the large tool as much as I'm able to.

 

-JD

[nickbe10]

I think you are stuck with it. It is trying to stage the tool, but by protecting the large tool pocket (I am assuming pockets either side are now disabled) it is turning the pocket "dedicated " to the large tool.

Some carousels have "dedicated" pockets and others are "random", and this could account for the differences between the machines.

Probably easiest to bypass  staging next tool after T35 in the post. You will still lose a bit of time but not as much.

We are looking at a 50T version of this machine. How do you like it other than the above problem?

[Leon82]

Some machines have an m code to initialize the tool table. You would need to reload them in the correct order but they would be in numerical order.

 

Over time the magazine is probably the most random it can be. Maybe a fresh start will help

[nickbe10]

I think you will get some delay here regardless of the type of tool changer unless the machine has a staging pocket separate from the storage chain........

[civiceg]

Are you sure pre-staging is not causing your issue? Seems to me that you are prestaging, then with the large tool going back into the carousel, it then rotates back to the large tool pocket and continues with the double tool change.  

You will always have the double tool change on a machine without an intermediate station, as it always puts the large tool back into the pocket with the adjacent pockets blocked out. 

[JeremyV]

On 8/31/2017 at 5:19 PM, nickbe10 said:

I think you are stuck with it. It is trying to stage the tool, but by protecting the large tool pocket (I am assuming pockets either side are now disabled) it is turning the pocket "dedicated " to the large tool.

Some carousels have "dedicated" pockets and others are "random", and this could account for the differences between the machines.

Probably easiest to bypass  staging next tool after T35 in the post. You will still lose a bit of time but not as much.

We are looking at a 50T version of this machine. How do you like it other than the above problem?

nick - as far as the machine itself there's always positives and negatives.  The machine we have is gear driven so we have a lot of torque, which is a nice thing.  Hardware wise, machine seems solid, software wise, I think it should be more user friendly.

We have a Haas VF-6 and a horizontal Mazak.... in terms of user friendliness, the HAAS wins, but again, the HAAS is 'okay' when it comes to hardware.  The mazak we have is a sweet machine; its fast, its easy to setup, and it has 10,000RPM.  The controls are a lil less user friendly, but anyone who runs Mazaks won't have this issue.  Plus, with a mazak you can do a great number of programming at the control.

I classify the doosan as non-user friendly, somewhat of a PITA to setup - at least with what we have. 

 

Seriously, 50 tools?!  The most we were able to get was 40....

On 9/1/2017 at 6:48 PM, civiceg said:

Are you sure pre-staging is not causing your issue? Seems to me that you are prestaging, then with the large tool going back into the carousel, it then rotates back to the large tool pocket and continues with the double tool change.  

You will always have the double tool change on a machine without an intermediate station, as it always puts the large tool back into the pocket with the adjacent pockets blocked out. 

We pre-stage tools on all of our machines.  Our previous mazak 655-60 had pre stage tools enabled, yet with large tool and empty adjacent pockets, the tool magazine remained motionless at the large pocket, even when the next tool was called up.  I liked this better vs the Doosan, because with the Doosan the magazine moves to the next tool instead of remaining where its at to save time.

The Haas we have functions the same as our old mazak.

 

Only 2 or 4 machines in the shop have random pockets.... the Doosan being one of them.  All the others are dedicated... and funny you should mention that because on of the old dinosaurs actually thinks the Doosan can be switched from random to ded, and I told him no so there was an argument about it till the repair guy came in and he asked him then said "my bad, you were right".   Random pockets are nice if you are only running 4 tools, you can place them side by side, which saves a tremendous amount of time if you are only doing one hole per part.

 

Thanks all for your feedback.  Looks like we're stuck with it.

[nickbe10]

1 minute ago, JeremyV said:

Seriously, 50 tools?!  The most we were able to get was 40....

No 50 taper.

Rigidity and stability are what we are after. The spindle carriage looks pretty solid in the brochure.....but I wanted an actual users opinion.

We have a Doosan lathe and the control is definitely not as user friendly as a Haas, however we strive for "post and go" here (and our first part guys are pretty good) so this is of secondary importance for us.

You should be able to bypass the tool staging for T35 using a Boolean statement and the nextool variable.  That will save you some time.

Have you done any post editing? If not it should be a good one to start on.

[JeremyV]

19 hours ago, nickbe10 said:

No 50 taper.

Rigidity and stability are what we are after. The spindle carriage looks pretty solid in the brochure.....but I wanted an actual users opinion.

We have a Doosan lathe and the control is definitely not as user friendly as a Haas, however we strive for "post and go" here (and our first part guys are pretty good) so this is of secondary importance for us.

You should be able to bypass the tool staging for T35 using a Boolean statement and the nextool variable.  That will save you some time.

Have you done any post editing? If not it should be a good one to start on.

I've done quite a bit of post editing, but nothing as complex as what you are suggesting.

 

The 50 taper machine is pretty solid as I believe they're a "big plus" spindle.  We've had the machine for 2 years now and while there were some minor issues with the tool changer itself, drifting, and guzzling too much oil, it has been solid and stable.  Still runs smooth.

I've ran a 3.875 OTM drill on the Doosan mill and the load was 50-60%.  Outside of the issues, machine performs remarkably well.

The side loading tool mag is nice, but it can be a pain and none of the guys liked it so we had to make a step platform so we can get into the machine and load tools from the front, which is also a pain. I've used it to remove tools as needed.

 

The tool changer issue was due to pockets being bad..... ( yes on a NEW machine )

The drifting issue we have happens when we shut the machine down all weekend then fire it up.  Even after warming it up twice, G54 home positions are never the same; all axis are off anywhere between .0005-.001 each - This is still an issue.

The oil guzzling was due to bad internal parts, which we just replaced.  It took us 2 years to realize that filling the way oil up daily was a bad thing.

[nickbe10]

4 hours ago, JeremyV said:

I've done quite a bit of post editing, but nothing as complex as what you are suggesting.

Thanks for the info Jeremy. Very useful.

I would encourage you to have a go at the post. The key here is to learn how to use the debugger. Have you got the MP documentation? You should be able to get it from your reseller.

I had a quick scan through the post after our previous exchange and it looks like it will all happen in one or more of the toolchange post blocks. (ptlchg_com, ptlchg0, ptlchg and ptlchg1002).

Figure out which variables you want to track and step through the post blocks and see how the variables change as the post blocks are read and mst importantly where the staging is actually posted as code (the debugger will tell you this). It should be pretty obvious which ones you need to "bypass" to avoid staging the tool "if nextool = 35". Once you get an idea of what you are after throw it up on the forum and you should get plenty of help. People like to see you have done some "homework" before you ask for help.

Good luck! Let me know if I can help. 

 

[JeremyV]

28 minutes ago, nickbe10 said:

Thanks for the info Jeremy. Very useful.

I would encourage you to have a go at the post. The key here is to learn how to use the debugger. Have you got the MP documentation? You should be able to get it from your reseller.

I had a quick scan through the post after our previous exchange and it looks like it will all happen in one or more of the toolchange post blocks. (ptlchg_com, ptlchg0, ptlchg and ptlchg1002).

Figure out which variables you want to track and step through the post blocks and see how the variables change as the post blocks are read and mst importantly where the staging is actually posted as code (the debugger will tell you this). It should be pretty obvious which ones you need to "bypass" to avoid staging the tool "if nextool = 35". Once you get an idea of what you are after throw it up on the forum and you should get plenty of help. People like to see you have done some "homework" before you ask for help.

Good luck! Let me know if I can help. 

 

I might tackle this tomorrow, will let you know.

Thanks!

[JeremyV]

On 9/6/2017 at 1:05 PM, nickbe10 said:

Good luck! Let me know if I can help. 

 

This was harder than i thought.

I was hoping a simple formula such as if t$ = 35, stagetool = 0 would work but nope lol.... not that simple =(

[nickbe10]

17 hours ago, JeremyV said:

This was harder than i thought.

Hey Jeremy,

They have me hopping here at the moment. It is New Part Introduction season and I have 16 machines to program for.

I should be able to take a closer look early next week and I will see if I can point you in the right direction.

[JeremyV]

17 minutes ago, nickbe10 said:

Hey Jeremy,

They have me hopping here at the moment. It is New Part Introduction season and I have 16 machines to program for.

I should be able to take a closer look early next week and I will see if I can point you in the right direction.

Np, but 16 machines?!   jeez.  Good luck!

and thanks,

[nickbe10]

23 hours ago, JeremyV said:

This was harder than i thought.

 

Hey Jeremy,

Had to go into a post to look at something so I couldn't resist.

In ptlchg_com, look for this line:

pbld, n$, "G43", *tlngno$, *tloffno$, pfzout, scoolant, next_tool$, e$

change to this:

	  if next_tool$ = 35,
	   [ 
	     pbld, n$, "G43", *tlngno$, *tloffno$, pfzout, scoolant, e$
	   ]
	  else,
	  pbld, n$, "G43", *tlngno$, *tloffno$, pfzout, scoolant, next_tool$, e$

This should also work:

	  if next_tool$ = 35, pbld, n$, "G43", *tlngno$, *tloffno$, pfzout, scoolant, e$
	  else,
	  pbld, n$, "G43", *tlngno$, *tloffno$, pfzout, scoolant, next_tool$, e$

I used the brackets just to make it easier to keep track of while editing.

So as you can see when the next tool is 35 it will not post the staged tool. Both output lines are the same except for the next_tool$ call. In all other cases it will.

N.B. I have not put this through any real testing! Make a copy of your post and try it out with the copy  in some of your programs where the tool is called at different places in the program so you are satisfied that you are getting reliable code in all situations.

I have an excellent first part machinist and I always tell him when I have done something in the post and he keeps an eye out until we are both satisfied there are no hidden bugs or loops somewhere.

Should be no problem here but it is always the time that you get overconfident and don't run proper checks that you end up getting bit, especially on something apparently "simple"

Good luck!

Edit: Thinking about it this might not give you exactly what you want, but let's try this first. Plan "B" will only require a slight modification.

[JeremyV]

I did some testing and compared codes.... you were right, it wasn't what I wanted but I did test the first code 2 ways:

      #pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$
      
      if *tlngno$ = 35,
	   [ 
	     pbld, n$, "G43", *tlngno$, pfzout, scoolant, e$
	   ]
	  else,
	  pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$

      #pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$
      
      if t$ = 35,
	   [ 
	     pbld, n$, "G43", *tlngno$, pfzout, scoolant, e$
	   ]
	  else,
	  pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$

Both work the way i need them to.  I went with the bottom code.

Now, hopefully the machine does not index, but if it does, there's something in the parameter that forces indexing.

 

(T35 = 8.0"  F-MILL )
N1620 (FINISH FACE - A270.)
N1630 G00 G40 G80 G90
N1640 T35
N1650 M6
N1660 S370 M03
N1670 G00 G54 G90 A270. X-.88 Y-8.
N1680 G43 H35 Z4. M08
N1690 Z.1
N1700 G94 G01 Z0. F50.
N1710 G41 D35 Y-3. F12.
N1720 Y3.
N1730 G40 Y8.
N1740 G00 Z4.
N1990 M09
N2000 G00 G91 G28 Z0.0 M05
N2010 G00 G91 G28 Y0.0
N2020 M01

Now, I need to try and figure out how to insert a previous tool command after M01 so the machine forces T35
to return to its dedicated pocket.  The issue is - a previously used tool will be sitting in the dedicated
pocket while T35 is in the spindle - I think this will be much harder as it has to be a parameter thing.

I have a few ideas, but not sure if they will work.  There is something I need to try first at the machine.  I know HAAS can tool change using the "P" code; Wonder if Doosan does the same.  Its just a matter of adding a similar formula.

EDIT: because tool 35 is in a dedicated pot, that pot will never change unless there is an issue with the hardware itself.

[nickbe10]

2 minutes ago, JeremyV said:

I have a few ideas, but not sure if they will work.

Hey Jeremy,

Good job...! I was going to suggest the following:

if  prv_next_tool$ = 35,

This might help get you going. I like this because it keeps you out of the "t" logic which is linked to other things like sequence numbers, so just safer to avoid any interference. I don't see any reason why yours shouldn't work though.

You should just be able to "call" without the M06 in the appropriate spot to stage tool.

 

if t$ = 35, pbld, n$, "T35", e$

The place you want to do this is in ptlchg$

      if mi10$=one, n$, *sm00, e$
      else, pbld, n$, *sm01, e$

The second line is where the M01 is output.

Let's see if you can figure it out. If not quote me again and I will try a couple of things to help.

Again test, test , test.....

Nearly there....!

[Henk]

• Before "T35", do an toolcall "T0"
• Then toolcall "T35", so "T0" is in pocket 35
• Run "T35"
• Again an toolcall "T0", "T35" is back in pocket 35
• Then call the next tool

[JeremyV]

1 hour ago, nickbe10 said:

Hey Jeremy,

...

if  prv_next_tool$ = 35,

You should just be able to "call" without the M06 in the appropriate spot to stage tool.

 

The place you want to do this is in ptlchg$

      if mi10$=one, n$, *sm00, e$
      else, pbld, n$, *sm01, e$

The second line is where the M01 is output.

Let's see if you can figure it out. If not quote me again and I will try a couple of things to help.

Again test, test , test.....

Nearly there....!

Hah, thanks!

I do have a massive list of mi10 items as part of a custom M00 line with comments so we do not have to keep typing them by hand - this way if we switch the same program to another machine, the same comment appears in the same spot.  It's just a matter of getting other programmers to remember it's there and how to enable it.  Coding the mi10 is the easy part - it may have to be the way to go -

 

A little background insight into our post history:  For about 18 years, we've had the same old posts until recently - 3 years ago - when CIMQUEST re-wote everything for us so the posts are fresh and new and updated.  Then a year ago we switched resellers, however the new reseller we were with now no longer supports mastercam >.<, so at the moment, I cannot be 100% sure if we are back with our previous reseller.  Communication with a forgetful boss is a PITA.

 

There were some codes i've had to add and modify on my own, including the creation of 2 new machine post files ( copy + paste + modify ), which turned out to be quite successful.

[nickbe10]

29 minutes ago, JeremyV said:

Hah, thanks!

No problem. I'll keep an eye on the thread if you need any more help, though you seem to be doing fine now.....

[JeremyV]

On 9/12/2017 at 10:48 AM, nickbe10 said:

No problem. I'll keep an eye on the thread if you need any more help, though you seem to be doing fine now.....

I've finally had some time to try out the other half of the formula.   I did do testing on the mill personally on Monday and I'm happy to say I've found what I need when T35 is called up:

(T35 = 8.0"  F-MILL )
N40 (ROUGH FACE - A0.)
N50 G00 G91 G28 Z0.
N60 T35
N70 M6
N80 S370 M03
N90 G00 G54 G90 A0. X-.88 Y-8.
N100 G43 H35 Z4. M08
N110 Z.1
N120 G94 G01 Z.01 F50.
N130 G41 D35 Y-3. F12.
N140 Y3.
N150 G40 Y8.
N400 G00 Z4.
N410 M09
N420 G00 G91 G28 Z0.0 M05
N430 G00 G91 G28 Y0.0
N440 M01 ( ***RETURN FACEMILL TO DEDICATED POCKET*** )
N450 P15 M06
N460 M01

So I went ahead and tried to add a boolean formula into the M01 section so the last 3 lines show up automatically when T35 is used, however the post file is setup in a way that mi10 needs to function on the next tool in order to get a custom code to post at the end of the previous toolpath.  I almost got it, but instead i did this:

if mi10$ = 98, n$, *sm01, "( ***RETURN FACEMILL TO DEDICATED POCKET*** )", e$, n$, "P15", "M06", e$, n$, *sm01, e$

 

[nickbe10]

1 hour ago, JeremyV said:

if mi10$ = 98, n$, *sm01, "( ***RETURN FACEMILL TO DEDICATED POCKET*** )", e$, n$, "P15",

Hey Jeremy,

I think I have an idea, but I am pretty jammed up at the moment.

Should be able to take a look later today. Will quote you again to let you know

So close I think we can do it....

Cheers

Nick

[nickbe10]

6 hours ago, JeremyV said:

if mi10$ = 98, n$, *sm01, "( ***RETURN FACEMILL TO DEDICATED POCKET*** )", e$, n$, "P15",

Hey Jeremy,

Show the code you want to see as well, (do you just need a T35 call where the brackets are?) and I will have a look first thing in the morning, been tough day......going home now

 

[JeremyV]

21 hours ago, nickbe10 said:

Hey Jeremy,

Show the code you want to see as well, (do you just need a T35 call where the brackets are?) and I will have a look first thing in the morning, been tough day......going home now

 

Sorry ya had a tough day.  Been busy myself as well.  First chance i got today to see this.... jeez.

Anyway, i'm not sure I understand what you are asking =\

[nickbe10]

18 minutes ago, JeremyV said:

Anyway, i'm not sure I understand what you are asking =\

If you had "T35" where your brackets are would it do what you need automatically, that is stage the tool at that point? 

[JeremyV]

On 9/29/2017 at 3:34 PM, nickbe10 said:

If you had "T35" where your brackets are would it do what you need automatically, that is stage the tool at that point? 

Well, no, it wouldn't do what I needed it to do automatically.  I think it has something to do with the way the post file is setup... I don't know if it needs to have something like "plast" or not.

The funny part is, when i used "first_tool", it only posted what I needed automatically for everything else, except T35.  I can get away with using mi10 option tho.

 

Thanks for everything tho