Integrex and MC

[DavidB]

Hi all

Is there anyone out there I can ask for help who is using MC to program there Integrex with a lower turret?

 

I'm having a difficult time trying to get this machine up and running using ISO programs.

 

I'm stuck with wait codes M950 and work offsets for every tool plane change.

 

I have plenty of questions so be warned

 

Brett must be sick of me

[crazy^millman]

Sorry David no lower turret here. But with out other machine that is a lower turret I have been able to do things pretty easily. The wait codes are still done by hand since Mastercam sucks at doing them, but 15 20 minutes on the machine and we get it going. Do you have problems with Master/Slave and surface speed? One thing I do not do it use canned cycles when I am doing roughing and finishing when using upper and lower turret. I long code it that way I can control it. Another tip when I am making my chains for upper and lower turret is taking dpeth of cut into account. I will mkae the lower turret chain smaller by the depth of cut and make sure the depth of cut on both is double what I am really doing since each one will be taking let say .1 per side I make sure the depth of cut is .2 on both operation and in reality they are cutting .1 per side. Need to keep horsepower in mind this is a smaller machine we have the dual turrets on so going for .4 per pass with a 25hp spindle is asking a lot on 32 rc material.

 

I will help any way I can with what I know, just don't have a lower turret on our Integrex.

 

As far as questions Go as Randy how many I have answered for him.

[Randy Morton @ Clem Industrial]

Lots! (And they are still coming....) =] You are wealth of knowledge Ron, and I do certainly appreciate that.

 

Did you see my pics in the O/T fourm?

[DavidB]

Thanks Ron

 

Can you help with Work Offsets?

This is from the Integrex Mark IV post processor programming guide from In-house.

 

quote:

---

Post,as with all other Mastercam posts,uses tool plane origin to out put work offset. You'll get G54G55etc. for 5-Axis milling. You get G53.5 for other work.

 

Anytime your offset number changes the post will give the appropriate G54G55etc. for 5-axis milling or a G50 shift if your just using G53.5.

 

YOU MUST SET YOUR WORK OFFSET IN MASTERCAM FOR EVERY OPERATION. Leaving it at the default -1 will force Mastercam to increment it with every new tool plane you use. This will give erroneous G54G55 output as well as G50 shift output!

---

 

What should I be doing so I dont get a G50 shift?

Or do you use a shift every time the T plane changes?

 

There is NO one running an Integrex with Lower turret in Australia with ISO code, so I am finding it very very hard to get help Down Under.

 

There are only 3 Intergrex's in Australia with Lower turret and the other two use Mazatroil only

[crazy^millman]

quote:

---

YOU MUST SET YOUR WORK OFFSET IN MASTERCAM FOR EVERY OPERATION

---

Well I think this explains it all. I see the part you have there as a basic 3 axis part or 4 axis part if you want to drill the holes using the lower turret. I would decide am I using G54 or G55 or such and that is what you need to set your workoffset to to maintain they are all the same for that operation. The series of Integrex you have is a lot different that the E series and handles everything more like a lathe than a mill. The E series does it more like a mill than a lathe in this since it works a lot easier with regards to shifts and such. I would try putting the fixture offset in the operations and see what type of posting I get.

 

If you got the PDF for the programming Manual and don't mind sending it my way it might help to understand how it handles these types of thing differently than the E series does. I also know the main Integrex guy at Mazak on the west coast and I don't mind contacting him and seeing what he says.

 

HTH

[DavidB]

I want to drill the holes with the Upper turret at C90 and C270.

 

The lower turret is for turning only no live tooling.

 

Ron you have mail

[crazy^millman]

Got to go pick my kid from school will look at this later and email you back what I think. I will also do a sample file like what you have drawn and want to see what happens when you post it with that post.

[DavidB]

Thanks Ron.

[crazy^millman]

David you got Mail with questions.

[crazy^millman]

I did this BMP for David I hope he does not mind me sharing for the benefit of others who may be having problems. Here is where and how to set the work offsets for a lathe:

 

HTH

[DavidB]

Ron if I put 1 for work offset it then askes for a Variable and outputs G53.5 with a G50 shift.

If I put 1 in more than 1 toolpath it comes up with a warning work offset allready used.

I'll double check Moday mate.

 

I must be doing something wrong

[Randy Morton @ Clem Industrial]

Primarily you would only get the 'offset already used' error if you are trying to force the offset on multiple tool planes. I hate that error, specially in a big program with 100 + tool paths cause you gotta look back thru them.

 

As Ron said with this acting more like a mill then a lathe, maybe this does not apply... but I set all my WCS's immediatly after I setup the part in MC, thus when I go the PLANES and NAMED VIEWS and change to a different plane (persay to drill your holes if that was defined seperatly) then it would automatically take the offset.

 

Again, I don't know how well this works for a machine that seems to be more lathe oriented then mill :S

 

Question for Ron; That tool file bmp you had above, is that from your tool file? Is that how you would get the eSeries head to be at 45 for OD turning instead of at 90? We have 45 deg holders for the OD tools as well as 90 deg holders and I don't know how to get MC to output B45 for those.

[crazy^millman]

quote:

---

If I put 1 in more than 1 toolpath it comes up with a warning work offset all ready used.

---

David this is that one that is not a problem. It is the same one you get in Mill when you are doing 4th axis work. Ignore it and post the code with a number in the workoffset and see what happens. Also David if you still get the G53.5 I would contact Brett and ask him to explain since the information on the Word.doc you sent says otherwise to that.

 

I think Randy means C-planes not WCS if you use WCS with this post you will not get indexes you will only get A0 moves. I always use C-planes not WCS to do my indexing.

 

Randy no that is not how I use the B head for tools like that. I got the correct information from someone at CNC here is a bmp of what I learned. That file was a sample file from lathe that I used for a lower turret example.

 

Any questions I will try to help.

[GoetzInd]

Also,

The forum over at www.integrexmachinist.com is very helpful for non programing integrex questions.

 

Mike

[DavidB]

When doing 4-axis mill work I use the Mpmaster and there is a switch Lock on first WCS if you do not select this on the first toolpath all following toolpaths the G54 will Increment by 1.

 

Do you use G53.5 or G54 to run your Integrex?

 

If you use G54 should I set all Tplanes to use a work offset of 1 in the WCS manager? Turning and milling tool planes?

 

Do you use G53.5 for the turning Ops?

 

So say I drill a hole using Top tool plane then another hole using Bottom tool plane should both planes have a work offset of 1?

Or better again I translate rotae the first toolpath 180 degrees.

[DavidB]

Ron I put a 1 for work offset in every tool.

 

I get this warning.

 

And MC still asks for shift variable numbers and there are no G54 in the posted code all G53.5 with shifts?

 

Here is the posted code

code:

---

 O0012 (INT0012A)

(PROGRAM NAME - INT0012A DATE=DD-MM-YY - 10-12-07 TIME=HH:MM - 07:47 )

(MASTERCAM - X)

(MCX FILE - T:PROJECTPROD_ENG_OP_SHEETSGOODRICH_JSFCH3123-0093 CH3123-0093_SWALLOW SHAFT .MCX )

(POST LICENSE - IN-HOUSE SOLUTIONS)

(T4 | 1.6MM CARBIDE DRILL | LEN. - 4. | DIA. - 4. )

 

(UPPER TURRET)

G109 L1

G28 U0. Y0. W0.

(G50 Shift Parameters Used)

(#501=)

(#502=)

(#503=)

(#504=)

(#505=)

(#506=)

(#507=)

(#508=)

(#509=)

(#510=)

(#511=)

(#512=)

 

N1

(T6 | 13.0MM CARBIDE DRILL | LEN. - 6. | DIA. - 6. )

(DRILL CENTRE HOLE UPPER TURRET)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G122.1

M950

M901

M200

G111

G53.5

T6 T004 M6 D006

G28 U0. V0. W0.

G97 S1500 M203

M248

M250 M212

G98 G0 B0. C0.

M251

G53.5

G0 G17 X100. Z20.

Y0.

M8

M153

G0 X0.

G0 Z10.

G83 Z-92.763 R0. F170. M210

G80

X200. Z10.

M9

M154

G28 W0.

G28 U0. Y0. M205

M951

M01

 

N2

(T4 | 1.6MM CARBIDE DRILL | LEN. - 4. | DIA. - 4. )

(DRILL)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G122.1

M952

M901

M200

G111

G53.5

T4 T-006 M6 D004

G28 U0. V0. W0.

G97 S4770 M203

M248

M250 M212

G98 G0 B90. C90.

M251

G53.5

G0 G19 X20. Z-4.

Y0.

M8

G87 X5.709 R3.75 F38. M210

G80

G28 W0.

G28 U0. Y0.

(DRILL)

M212

G0 C270.

M250

G0 B90.

M251

G19 G0 X20. Z-4.

Y0.

G87 X5.709 R3.75 F38. M210

G80

M9

G28 W0.

G28 U0. Y0. M205

M953

M8

 

N3

(TRANSFER WITH PUSH)

M953

G28 U0. Y0.

G28 W0.

G53.5

M202

M250

G0 B0

M251

M513 (UN SYNC SPDL'S)

M200 M300 (MILL MODE SPDL'S 1&2)

G0 C0. (C0 SPDL 1)

G110 C2 (SWITCH C AXIS CONTROL OVER TO 2ND SPDL)

G0 C0. (C0 SPDL 2)

G111 (CANCEL G110 MODE)

M306 (CHUCK OPEN SPDL 2)

G110 B2 (CROSS CONTROL TO 2ND B AXIS)

M540(TRS-CHK)

(PICK OFF POSITION)

(#601=)

G00 B-[#601-0.] (MOVE 2ND SPDL TO PICK OFF MINUS RAPID DIST)

G112

M508

G98 G31 B-[#601-0.] F100 (MOVE 2ND SPDL TO PICK OFF MINUS APPROACH DIST)

G31 B-[#601] F5 (MOVE 2ND SPDL TO PICK OFF)

G112 M509

M541

M307 (CHUCK CLOSE 2ND SPDL)

G111

G4 X3.

M206 (CHUCK OPEN MAIN SPDL)

G4 X2

G110 B2

G00 B-[#601-#600]F80.

G111

 

M30

 

(LOWER TURRET)

G109 L2

(T9 | STOP | DIA. - 9.)

(T1 | 0A ROUGHER LOWER TURRET | DIA. - 1.)

(T2 | 55J ROUGHER LOWER TURRET | DIA. - 2.)

(T6 | 3.18 GROOVE LOWER TURRET | DIA. - 6.)

(T3 | 55K FINISHER LOWER TURRET | DIA. - 3.)

G28 U0. W0.

 

N1

(T9 | STOP | DIA. - 9.)

(STOP OUT)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G21 G123.1

M901

M202

G53.5

T009009

G28 U0. W0.

G50 W-#500

G18

G50 S6000 R2

G96 S90 M04 R2

G0 X0. Z10.

M8

Z0.

Z10.

M9

G111

G28 W0.

G28 U0.

M01

 

N2

(T1 | 0A ROUGHER LOWER TURRET | DIA. - 1.)

(ROUGH FACE)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G123.1

M901

M202

G53.5

T001001

G28 U0. W0.

G18

G50 S6000 R2

G96 S140 M03 R2

G0 X35.75 Z.05

M8

G99 G1 X-1.6 F.3

G0 Z1.05

(ROUGH OD)

X29.843

Z4.6

G1 Z2.6

Z-110.292

X31.75

X34.578 Z-108.877

G0 Z4.6

X27.936

G1 Z2.6

Z-110.292

X30.343

X33.171 Z-108.877

G0 Z4.6

X26.029

G1 Z2.6

Z-8.127

G18 G3 X26.462 Z-8.375 R.85

G1 X27.642 Z-9.397

G3 X27.87 Z-9.822 R.85

G1 Z-11.6

Z-19.845

Z-110.292

X28.436

X31.264 Z-108.877

G0 Z4.6

X24.121

G1 Z2.6

Z-7.95

X24.99

G3 X26.462 Z-8.375 R.85

G1 X26.529 Z-8.432

X29.357 Z-7.018

G0 Z4.6

X22.214

G1 Z2.6

Z-7.95

X24.621

X27.45 Z-6.536

G0 Z4.6

X20.307

G1 Z2.6

Z-7.95

X22.714

X25.543 Z-6.536

G0 Z4.8

X18.4

G1 Z2.8

Z-7.95

X20.807

X23.636 Z-6.536

M9

G111

G28 W0.

G28 U0.

M01

 

N3

(T2 | 55J ROUGHER LOWER TURRET | DIA. - 2.)

(ROUGH OD STEP)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G123.1

M901

M202

G53.5

T002002

G28 U0. W0.

G18

G50 S6000 R2

G96 S120 M03 R2

G0 X34.442 Z-19.623

M8

G99 G1 X30.442 F.2

X26.462 Z-23.07

X26.391 Z-23.132

Z-105.6

X29.219 Z-104.186

G0 X30.891

Z-22.699

G1 X26.891

X26.462 Z-23.07

X24.839 Z-24.476

Z-105.6

X27.668 Z-104.186

G0 X29.339

Z-24.043

G1 X25.339

X23.288 Z-25.819

Z-105.6

X26.116 Z-104.186

G0 X27.788

Z-25.386

G1 X23.788

X21.736 Z-27.163

Z-105.6

X24.564 Z-104.186

M9

G111

G28 W0.

G28 U0.

M01

 

N4

(T6 | 3.18 GROOVE LOWER TURRET | DIA. - 6.)

(ROUGH GROOVE)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G123.1

M901

M202

G53.5

T006006

G28 U0. W0.

G18

G50 S5000 R2

G96 S90 M03 R2

G0 X29.47 Z-18.795

M8

G99 G1 X21.656 F.07

G0 X29.47

Z-16.

G1 X21.536

G0 X29.47

X30.159

Z-15.101

G18 G2 X27.47 Z-15.833 R2.

G3 X26.77 Z-16. R.45

G1 X21.536

X22.275 Z-16.369

G0 X29.47

X30.159

Z-19.694

G3 X27.47 Z-18.962 R2.

G2 X26.77 Z-18.795 R.45

G1 X21.656

X22.395 Z-18.426

G0 X29.47

(ROUGH)

G18

X31.47

Z-26.845

G1 X21.556

G0 X31.47

M9

G111

G28 W0.

G28 U0.

M05

M950

M01

 

N5

(T3 | 55K FINISHER LOWER TURRET | DIA. - 3.)

(FINISH OD)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G123.1

M951

M901

M202

G53.5

T003003

G28 U0. W0.

G18

G50 S6000 R2

G96 S120 M03 R2

G0 X13. Z2.

M8

G99 G1 Z0. F.1

X17.2

G18 G3 X18. Z-.4 R.4

G1 Z-7.9

G2 X18.2 Z-8. R.1

G1 X25.49

G3 X26.183 Z-8.2 R.4

G1 X27.363 Z-9.222

G3 X27.47 Z-9.422 R.4

G1 Z-11.2

Z-19.445

Z-25.342

X30.298 Z-23.927

(FINISH OD)

G18

G0 Z-20.557

X28.363

G1 X27.363 Z-21.423

X26.176 Z-22.451

X21.336 Z-26.324

Z-99.8

X24.164 Z-98.386

G0 X100.

M9

G111

G28 W0.

G28 U0.

M01

 

N6

(T6 | 3.18 GROOVE LOWER TURRET | DIA. - 6.)

(FINISH)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G123.1

M901

M202

G53.5

T006006

G28 U0. W0.

G18

G50 S5000 R2

G96 S90 M03 R2

G0 X31.47 Z-19.245

M8

G99 G1 X27.47 F.07

G18 G2 X26.67 Z-18.845 R.4

G1 X21.556

G3 X21.336 Z-18.735 R.11

G1 Z-16.925

X21.831 Z-16.678

G0 X31.47

G18

Z-15.55

G1 X27.47

G18 G3 X26.67 Z-15.95 R.4

G1 X21.336

Z-17.676

X21.831 Z-17.924

G0 X31.47

(FINISH SHOULDER)

G18

G50 S6000 R2

Z-26.795

X30.29

G1 X26.29

X21.556

G18 G2 X21.336 Z-26.905 R.11

G1 X25.336

G0 X100.

M9

G111

G28 W0.

G28 U0.

M05

M952

G0 G28 U0

G28 W0

T000001

G0 G28 W0

M30

 

---

Ron from the Programming guide.

quote:

---

Work Offsets

 

Post, as with all other Mastercam posts, uses tool plane origin to output work offset. You’ll get G54/G55 etc. for 5-axis milling. You get G53.5 for all other work.

---

G54 only with 5-axis?

You get 53.5 for ALL other work?

 

Maybe a G50 shift is how it is meant to work?

 

[ 12-09-2007, 04:18 PM: Message edited by: DavidB@Rosebank-Engineering ]

[crazy^millman]

Ok so is G53.5 a work plane shift? My Integrex post does not work this way. I have G54 for all of my 2,3,4,5 axis output. I do get a G43.4 for 5 axis and G68 which is the work plane shift, but it is all relative to the G54. I really have no answer for the G53.5. What happens when you run the code? How does the machine act? Doe it alarm? Does it make crazy moves? What does the book say about G53.5 and how it works? I understand the post outputting parameters, relative to using a G50 shift which you are not doing. Also what does the G123.1 mean for your machine?

[DavidB]

G123.1 X-axis radial command OFF

G53.5 Selection of MAZATROL Coordinate System.(Series T)

 

I dont understand why I get a G50 shift for toolpaths using Top and Bottom Tool plane but I have toolpath using the right side tool plane and it posts out with a B0 and does not ask for a shift variable.

 

[Greg Williams]

Perhaps a quick email to Brett may be the best solution

[DavidB]

Hi Greg how's things?

 

Brett has been very helpful but in fairness to him I wanted to try find out as much as I could before I bother him again.

 

It's really only Bretts need to help if it's post related, not if I dont know how to use the machine and MC

[Post dept]

All,

 

A short explanation of how work offsets work follows:

 

If you do not set a work offset value in Mastercam (leave it as -1), Mastercam increments the variable called workofs$ for every new tool plane it encounters. So, you're effectively telling the post you want a new offset for every new plane. For some posts, that means G54,G55,G56, etc. The integrex works a little bit differently. For the Mazatrol side of the control you've only got 1 or 2. G53(.5), and on the Mark II you could get a P1/P2 option. So, when you want to chagne to a new work offset, you need to do a G50 shift. Every time the post sees a new work offset, it sees asks for that shift variable then outputs accordingly. Hence the message YOU MUST SET YOUR WORK OFFSET IN MASTERCAM FOR EVERY OPERATION

 

I encourage people to set all ops on the main to work offset 0, and all ops on the sub to work offset 1. this can be done through the view manager as Ron had shown earlier.

[DavidB]

Thanks Brett

Hopefully I'll make some swarf today.

[DavidB]

Got the machine moving today.

Just got to get the the transfers working.

 

Brett you've done a great job of making the post.

 

Thanks to all for there help.

 

The questions will still be coming we have some fancy 5-axis work coming up for the Integrex.

[Ron Branch @ Verisurf]

Anytime you need anything David you got my email.

 

 

Yes Brett has done a very good job with these Post, as well as everyone else at IN-House that helped it get to where it is.