Mastercam for Integrex 300y

[Harryman]

Good day fellow Mazochists.

 

We are currently running the first 300Y in North America, with considerable success. We have been using Mazatrol (not the source of success) and hand written macros. We tried to find a usable CAM system very early on, but I tired of being the guinea pig for everything, and sort of sat back a couple years to let others in on the fun.

 

Dave, the good administrator of this board, is working on a post for us right now. He has been a truly good sport. There are a couple issues that I'd like to raise here though, that I'd like other users to comment on to provide support for, or not, some features that I pose should be included in a new post that CNC Software promises to write some day.

 

1 Let's lose the gearhead lathe bagage and use G125, some folk seem to have G124, for milling and drilling at all B angles including 0, 90, and 270 degrees. (I don't have a sub spindle so I haven't tested G125 at 270. I will post the needed repair to the Mazacode for 90 degree case if there is interest.) This will allow a single Tool Data Page discription for a drill or end mill rather than two or three. It will also eliminate the need to use "cross drilling" G codes, such as G87 for "cross peck drilling."

 

2 Chip break pecking anyone? Mazak provided P10 bit 6 to toggle G83 between chip break pecking and full retract drill pecking. Now I know I'm the only one on earth that wants to make that call in the program rather than a machine parameter, but I wrote up a little user macro that emulates a chip break peck (G87 on most mills right?) and if we can get CNC to force output of G81 (unused on our Integrex, so used by me for my macro) at each position, we can have something close to mill style chip break pecking via G code rather than long code. I'll even post my macro. And combined with sugestion #1 only one aliased G code is required. Huh?, Huh? (insert Marge Simpson Smiley here)

 

Enough typing for now. I've got a few other ideas if anyone is interested in this train of thought.

[McRae]

It has been experienced that Mazak is not interested in user feed back - but group theropy is a good thing.

 

Internal Peck - lets see... G73 on the fanuc mills, but reading thru the manual (Remember legacy lathe) G73 is a lathe volume removal cycle. We have had the similar thing here where on the Fanuc 7M, the canned cycles are actually user macros anyway, so your personal creation method was the only solution there.

 

Was mazak forthcoming with coding assistance on this?

 

I was successful at getting the probe to print to an internal file on the machine's harddirve with the assistance of Mazak. Any one interested, send a message and I will forward the document.

[chris m]

Andrew

 

I got your message yesterday, I apologize for not responding but it is very busy here and I have been out on the floor for a couple days running a VMC trying to pump out a rush job. I appreciate your offer, right now the future of my machine is unknown; I'll know what the story is in a couple of weeks, I think.

 

C

[Harryman]

I surely know better than waste time asking Mazak for assistance on something like this. I wrote the code. And since it runs as a sub program, rather than as a true G code, it must be called at each position. The pecking parameters, however, are common variables and so are more or less modal giving you one place to change peck depths and simple places to resume drilling any of many holes, something that is much tougher if you are running long code to peck many holes.

 

I'm simply suggesting that if we can get Mastercam to aggree that this is a reasonable workaround for a Mazak omission, we can have a way to chip break peck without long code, or the Mazak solution, programmed parameter change.

 

The macro can be aliased to any available G code via K81-K88.

[McRae]

Harry,

 

Send the code along to me as I am interested. I was going to suggest the aliased method of calling it - what are your input parameters? What variables in the code are you using?

 

Look forward to more!

[Harryman]

The variables passed are: D, F, Q, R, Z, M,

 

It behaves exactly like G83 and uses the same variables. I set common varibles from the original locals. G83 requires Q at each location ? ? so any post processor already forces Q output. The only added burden to post processor writer is to force G(alias) in addition to Q.

 

I wrote the macro assuming that it would always be posted by CAM and therefore did not include additional positioning capability, or repetetive function. It just breaks chips.

[Jack Mitchell]

Friends,

 

It has been 14 years since I did this. I will try to search for some factual details during the weekend. – This was done on the M32 control.

 

Mazatrol is nothing but macros that remain out of site:

 

I recall that I had to push MF1 (Miscellaneous function key) plus another number IE:8 (Just can't seem to remember)

I powered down - I powered back up - The only programs that became available were all the macros in the control, no Mazatrol programs; in fact I could only address in Eia since the whole interface was gone.

 

I will have to do some serious research to see if I could do the same to the 640M & 640T Fusion controls.

 

What I am getting at here, is I believe your customization request is right there all ready.

 

I too would be very interested in see some of this work that you guys are delving into.

 

Regards, Jack

 

[ 02-05-2003, 12:54 AM: Message edited by: Jack Mitchell ]

[McRae]

Jack - We can play here if you want...

[Harryman]

Are y'all suggesting that you think you could get the macro into the beast's belly where it would behave like a "real" G code?

 

On my machine, K81 is set to Code 130 and Number 100009114 which tells me that G130 is only half "real" and Mazak stole one of the "user" G code assignments to run G130.

 

Find 100009114 and you've found where to implant the chip break G code.

[McRae]

Harry,

 

That is exactly what we are suggesting.

[Part Factory]

Harry:

 

I quote Mazak's response to me:

"" This information is proprietary and cannot be accessed by customers. This information is not required for proper operation and does not inhibit the customer from using the machine to its fullest capabilities. ""

 

From what I have read in your responses the Integrex has many customers that cannot use it's full capabilities. I hope these hidden G-codes are the "pot of gold" that makes the machine buggy. Also, I hope that there is no connection to the mysterious 3-digit g-code mentioned in the documentation because of its nonexsistant technical description in the manuals.

 

Oh Ya

Can anyone out there explain to me why Mazak makes such a capable machine with the most uncapable programming access on the planet?

[Jack Mitchell]

Here is a simple Mcode.

 

M200 links via the parameters accessing P9000 which is available in my files directory

 

G91 G28 XYZ

G90

M99 or M02?

%

 

Create an Mcode to grab the Eia program and execute this with Mastercam or Mazatrol.

 

I have indeed been inside the beasts belly, the way I got in was I used two V15's with M2 controls. The controls were both large swing pendants - I could actually work two controls simultaneously while operating one machine; the M2 has all the options that you had to pay extra dollars, the M32/T32 controls used eproms or chips to stop the spread of the freebie features.

 

I was really curiuos on how it controlled selecting a pilot drill automatically, this fascinated me.

drill .1

drill .11

drill .12 thru 2" in .01 increments etc!

I did this for every single automatic cycle within the M2 control - from here I attacked the 500 some parameters that were sort of glazed over in the parameter manuals as well as the 300 that are not published.

 

As I was talking with a service technician one day -I explained how I attacked learning all this stuff; the service tech was blown away and told me he had never seen anybody figuer this stuff out before. Turns out he walked out of Yamazaki Japan with the all the goods, he showed me some tricks which is how I learned to tweak the control.

 

I rarely throw anything away- especially something that took about nine months to comprehend and learn; It all happened about twenty years ago so give me some time this weekend to try to find this handwritten info.

 

Regards, Jack

 

[ 02-05-2003, 01:25 AM: Message edited by: Jack Mitchell ]

[Jack Mitchell]

Guy's,

 

I cannot stress this enough BE VERY CAREFUL when adjusting parameters - this is why Mazak will not release this information and why they will not satisfy your questions - it's very dangerous and very propietary.

 

I'm sure that Dave Thompson would vouch for the difficulty of mastering a post for these machines - it's all math,logic, and hundreds of hours of refining.

 

Regards, Jack

[Harryman]

Atta Boy for that extreme parameter detective work, Jack. (insert Hat's Off Smilely here)

 

I hear you on the complexity for the post writer, hence this thread on losing the diametrical X baggage for milling, eliminating duplicate G codes for unique B angles, and providing a chip break G code.

 

If we can get the train of thought away from the cross drilling mentality of the gearhead live tool lathe days, then it's a short hop to use G130 for helical work in all directions rather than long code. (I'm not a fan of the long code)

 

Offset tweaks for accuracy on multiple features using a single tool ,horizontal, can be accomplished with G50 shifting. G50 shifts operate cumulatively and are cancled by G53 or reset so they are pretty safe to use and can be used in combination with the G50 calls made by G125.

[Jack Mitchell]

I’m sorry, but I cannot recall which member posed the question regarding a G73 high speed peck requirement on the Mazak Integrex.

I believe this machine to be primarily a turning center with the adage of live tooling as well as the inclusion of two additional axis. The conflicting problem is that Fanuc & Mitsubishi allocated the G73 cycle as a pattern repeat for turning centers – who could know that more than 30 years after establishing the standards that there could be problems down the proverbial road.

 

NOTE: For the Mazak M32 control only (Mazak Fusion 640M will follow this shortly)

The means into the belly of the beast is as simple as the following jpegs.

Please note that I indeed took these pictures, and then repeated the process without any loss of parametric information or original saved programs.

 

O108 input a 1 in here

Power down (just at the control)

Power up

Now just look at all of those macros that are available instead of the usual programs

 

O108 input a 0 in here

Power down (just at the control)

Power up

Hey your programs have all returned and the macro’s are once again safe from view.

 

Now if you wish to take fate by the horns then by all means edit the existing macros, this will save your edits.

An extreme word of caution is in order here: The programmer that created these macros was indeed brilliant for the mid 1970s and this is well before any form personal computing was available to the general public – please proceed with the utmost caution.

 

You might wish to address my post immediately following this one for a more preferred method.

 

Regards, Jack

 

 

 

 

 

 

 

And finally back home safe and sound as I stated.

 

Notice that 101 of 102 records were used, the missing one is required for MDI operation. It's as if Yamazaki will not allow the inclusion of any further bytes - at least on my control.

 

[ 10-05-2003, 06:37 PM: Message edited by: Jack Mitchell ]

[Jack Mitchell]

Aahh- the ominous machine parameters that Yamazaki will never explain or publish

 

NOTE: For the Mazak M32 control only (Mazak Fusion 640M will follow this shortly)

 

Access the “J” machine parameter screen

Goto J61 and enter 9000

Goto J62 and enter 200

Then exit the parameter pages

 

Create a new EIA program number 9000 and keep this in the program file on your machine.

 

M09

G91 G28 XYZ

M99

%

 

The Mazatrol cowboys know full well how they always have to manual program with a duplicate tool and an M00 in the second or third unit – otherwise the machine will keep cycling on continue “Y” it’s how we pre-stage the first tool for efficient machining.

 

J61 tells the control which program to execute.

J62 tells the control which “M” code is attached to it.

 

The beauty is that M200 will function via MDI, Mazatrol, or EIA.

 

I always end a production job with M200 and "Y" for continue; there is no macro for the beginning of the program since knowing which tool to preload is never consistant enough to warrant writing one.

 

I do the same with parameters J57 and J58 as well – used as a simple Mcode call instead of imbedded subroutines. (I know that M200 wasn’t currently in use but I could call this M500 for all that it matters).

 

I recall that some individual has written a comprehensive macro for peck drilling on an Integrex – my suggestion is to use it as a simple Mcode that is available whether in Mazatrol or Mastercam.

 

There are probably five or six additional “J” parameters readily available as well; it’s just that I have never required more than these two.

 

I realize that 9000 also echoes within the screen shot - don't be concerned about this since the Mazatrol macros are independant of the program file numbers.

 

Harry - If you use this concept then the only condition is to be sure the required macro always remains present in the PROGRAM file directory and then simply use the miscellaneous function from within Mastercam; I'll have a look at the 640M tomorrow afternoon.

 

 

Regards, Jack

 

[ 10-06-2003, 10:43 AM: Message edited by: Jack Mitchell ]

[crazy^millman]

Yeah Jack the 1131 alos if you hit the far left button (nobody called me on my joke here yet didn't put the true way or did I) when on the paramete page you have access to those place most dare not go. I have also twaeked thses parameter when I had a 4th axis on my VTC-30 wit hthe PC-Fusion comtroller on it. I will also say that you can print out the macro code on a PC-Fusion if you use the DNC cable to send programs back to a copmuter. It will print out the complete Mazak program as the complete code seen by the Machine that Mazatrol is using. I will also tell you that you can get inot the Ladder program also and do thing in there though Mazak about hit the freaking roof when I told them some of the things I did.

 

I did hear of one guy taking the Hard drive out of a PC-Fusion and copying it over to a PC to play with the code off the Machine. I know it will work cause I took and copied alot of the stuff and was able to play with certain things. It just takes some work knowing what the keyboard key do the control functions. I had to leave alot of my Mazak stuff back in Florida and cant go back and see my notes.

 

I really know this is a crazy thing to say but I really miss the Mazak Machines.

 

Crazy Millman

 

[ 10-06-2003, 09:27 AM: Message edited by: Millman^Crazy ]

[Harryman]

Good morning Jack.

 

That's some very interesting xxxxhing. I never really wanted to get that far in. Now that you have found the path though... Perhaps one could just analyse the G83 macro and copy the section that runs in chip break mode when P10(bit6)=1 and then call it with an unused G code.

 

Note to Mazaspy: when you see your customers discussing this level of modification in order to enable a simple function (chip break pecking) that virtually any modern machine builder provides via simple G code, rather than Mazak's machine parameter method on the Integrex, you have a chance to earn some positive ink by chugging off to the drawing board and making it work then offering it to all customers. TAKE THE HINT!!!

[Harryman]

Jack, I took a bit more time to read your post tonight. We have the early fusion 640 MT control. It's facinating that you got behind the looking glass into the Mazatrol macros.

 

I did succeed in writing a usable chip break peck macro and aliasing it to G81. Dave set up the post to call it, and while it's not an elegant solution, it works and is easier to edit than long code. On the fusion control, the program goes into a windows file that I can't remember the name of here at home. It loads at power up.

 

Dave also set the post up to use G125 at B90 so we did indeed get rid of the Cross Drilling baggage. We use G83 for drilling at all angles with a single horizontal tool definition, and G81 for chip break pecking at all angles, and G84.2 for tapping at all angles.

 

We also have turning working with the B Axis at positions other than 0 and 90. That's working sweet. You define the tool shank angle in the tool parameters, and it appears angled on the library thumbnail when you select library tools. When you create a turning operation, the post reads the angle and sets B. You need to have a tool data page offset that can be addressed via 8 digit T call with offset values valid for the tool in the angled position. Piece O'Cake

[Jack Mitchell]

Millman,

 

The way into the Fusion differs from the M32 control.

 

I know the "O" parameter screen exists but alas, I do not know the method in, any suggestions would be appreciated.

 

There is a screen shot in a parameter page only and I do not think Mazak would be receptive to my questions on this matter; I do know somebody else who likely shares my enthusiasm regarding this but I don't think I can get together with him for a few months.

 

Let me know if you can help.

 

PS: Just pick a couple of available "J" parameters that are at zero - (towards the higher end numbers) there are lots of sets available for customized Mcodes as I stated in an earlier post.

 

Regards, Jack

 

[ 10-07-2003, 11:26 AM: Message edited by: Jack Mitchell ]