DMU100T Help with moves between 3+2 and 5 axis.

[crazy^millman]

Okay so TK-32 is who I am helping out here. They have a DMU100T machine with a Mill-Plus control. When the machine is doing 3+2 is is running the posted code fine. Switch over to 5 Axis and all things break loose. The post uses a L1=1 between the switch from 3+2 to 5 axis. At the start of the 3+2 you have a G7 A5=0 and B5=XX.XXX C=XX.XXXX L1=1 and that seems to move the machine to the 3+2 position and if is off and running. Now you switch over to the 5 axis tool path and it goes to the machine zero position for all axis because of the L1=1 which is puzzling because of why? Anyway then the 5 axis move after this is just a simple C axis move of the index table to put the machine in place for the next 3+2 work. No dice it will crash the machine big time. So anyone with experience with these mind commenting on what you have seen for code between the 2 types of operation that was effective for you. Here is a snippet of the code from the start.

 

%PM0001
N1
N100 ( 240550-1 B )
N110 ( DATE- 23-06-12  TIME- 11:22 )
N120 ( 1/2 BULL EM .125 R	DIA.-.5 )
N130 G70
N140 G54 I1
N150 G74 Z-.1 L1
N160 G7 L1=1
N170 T1 M6
N180 M57
N190 M57
N200 G7 A5=0. B5=-83.035 C5=-45.171 L1=2
N210 G90
N220 G0 X1.673 Y.1994
N230 S10000 M3
N240 Z4.
N250 Z3.925
N260 G1 Z3.9 F200.
N270 X1.6743 Y.1997 Z3.886
N280 X1.6781 Y.2007 Z3.8724
N290 X1.6844 Y.2022 Z3.8598
N300 X1.6928 Y.2043 Z3.8487
N310 X1.703 Y.2068 Z3.8393
N320 X1.7148 Y.2097 Z3.8322

 

Then here is the transition from that 3+2 to the 5 axis as it is called from the posted code.

 

N5930 X2.2209 Y-1.2294 Z2.1799
N5940 X2.2162 Y-1.2226 Z2.1909
N5950 X2.2127 Y-1.2176 Z2.2032
N5960 X2.2106 Y-1.2145 Z2.2164
N5970 X2.2099 Y-1.2135 Z2.2301
N5980 Z3.725
N5990 G0 Z4.
N6000 G7 L1=1
N6010 G0 X-2.6022 Y2.9007 Z2.1609 C-45.171 B-83.035
N6020 G1 X-2.966 Y2.5542 Z2.223 C-42.362 B-82.459 F120.
N6030 X-3.2817 Y2.1623 Z2.2868 C-39.05 B-81.804
N6040 X-3.4134 Y1.9471 Z2.3189 C-37.085 B-81.43
N6050 X-3.545 Y1.7319 Z2.3511 C-35.116 B-81.065
N6060 X-3.6481 Y1.5008 Z2.383 C-32.769 B-80.644
N6070 X-3.7511 Y1.2696 Z2.415 C-30.416 B-80.239
N6080 X-3.8234 Y1.026 Z2.4461 C-27.605 B-79.778
N6090 X-3.8954 Y.7822 Z2.4772 C-24.785 B-79.341
N6100 X-3.9218 Y.6141 Z2.4971 C-22.552 B-79.013

 

So the question here is why would it be so far to crash the machine? I am digging into in, but again if someone with experience with these machine has suggestion I am all ears for your help or suggestions. Thanks in advance for help or suggestions you may have.

[Guest SAIPEM]

G7 L1=0 will reset the coordinate system but will not move any axis.

 

G7 L1=1 will move the table & reset the coordinate system.

 

G7 L1=2 moves all 5 axis simultaneously but keeps the tool in the same relative position.

[TK-32™]

Thanks Saipem, I'm going to try that tomorrow

[crazy^millman]

Well I thought we tried all 3 combinations, but it was long day so maybe Monday TK and check it out and see what helps it run. His reseller is working on the post as well so that should help him out. Saipem thanks for the response it is appreciated. Did you run top map for both 3+2 and 5 axis or a combination of both?

[Guest SAIPEM]

Well I thought we tried all 3 combinations, but it was long day so maybe Monday TK and check it out and see what helps it run. His reseller is working on the post as well so that should help him out. Saipem thanks for the response it is appreciated. Did you run top map for both 3+2 and 5 axis or a combination of both?

 

 

It's been a long time since I've touched a DMU.

I'm going by memory.

 

I did notice in your first example you have L1=1 and then a L1=2

 

Your second example doesn't have that

Change the second example to use an L1=2 and see what you get.

[crazy^millman]

Thanks Saipem. TK is getting deep into 5 axis land so this is all good stuff for him to try.

[Watcher]

Ron,

 

I wrote a post for these 4-5 years ago... all bells and whistles...

 

Add a G174 in between the modes... G174 will retract all linear axes along the current tool axis until a software limit is reached to whichever axis gets there first... it's always along the tool axis (Z+)...

 

In your shoes I'd also add a G93 C3=1 (It can be A1=1 B1=1 or C1=1 but usually only the C axis is limitless) to reset the C axis so you can have the shortest move... the thing with G7 / Cycle 19 is that they are cumulative functions... that is, after a bunch of G7 your C axis can be at let's say 1082 degrees... when in fact it is at 2 degrees... G93 C3=1 will rewind the C axis to a value in between 0-360 so it will put it at 2 degrees in the axis coordinates without moving the axis... this way if your first C axis move in multiaxis mode is let's say 3.572 degrees C will rotate only 1.572 degrees and you won´t get a full rewind that can crash the tool... A Mazak dude like you is not used to go beyond 360 right? (Just kidding)

 

In my post, if I remember correctly, between the modes I had this:

 

G7 L1=0

G174

G93 C3=1

G141 L2=1 ;5 axis mode active (L2=0 Shortest moves / L2=1 Absolute)

...

 

I noticed your post is not using G141 but rather the computed XYZBC coordinates... well... not sure if I would do it this way... in G141 mode the control has better performance as it uses a second dedicated processor.... in G141 (TCPM) you can have your zero point everywhere you want and the control will compensate it for you... without it sometimes you are tied to having your zero point physically defined in the center of the C axis rotation...

 

One tip with G141: Don't use I1= J1= K1= as the tool vectors... rather, set the post to compute B and C and to output XYZ for you... XYZ don't change and can be exactly what they are in the NCI... when you use I1 J1 K1 in Millplus the controller goes faster to process the data but it will make all decisions for you as the post won't know the axis limits... when you use A B C you can set the post to check the position of the axes and if any limit is being reached or unexpected rewinds are happening... by checking the B / C angles you can have an idea of what is going on in the tape and have some safeguards on your end...

 

For example, if for any reason your program reach the limit of the C axis (99999.999) you can write a logic to check the position of the C axis for each G1 line...

 

If current_c > 99999.0 Then

sav_current_x = current_x

sav_current_y = current_y

sav_current_z = current_z

sav_current_b = current_b

sav_current_c = current_c

safety_distance = 10 ;Write your safety distance value here....

 

Print "G174"

Print "G40"

Print "G7 L1=0" (Not needed in multiaxis but helps if you re-start in the block search mode)

Print "G93 C3=1" (Reset the current C axis value to a value between 0-360)

current_c = mod(sav_current_c)

 

goto rapid sav_current_c

goto rapid sav_current_b

goto rapid sav_current_x,sav_current_y

Print "G141 L1=1"

 

goto rapid sav_current_z + safety distance

goto feed sav_current_z

 

Restart the cut from here...

 

Sorry for the pseudocode above but I really forgot how to code in MP Language... (APT dude in the past 7 years)

 

One benefit of G141 is that your post does not have to do any computation (Thus the post-processing is faster): The XYZ coordinates in the program are the same ones is the Mastercam NCI, and this is also true for the tool vectors... The control does the whole thing for you... Also, small changes on the pivot distances / calibrations won't require a new code... changes in the tool length does not affect the code either...

 

In G141 with IJK... they become I1 J1 and K1 but in milesimal format as far as I remember... if for now you find it hard to compute B and C from these vectors, you can make the post just to simply spit XYZIJK out to the control in the G141 L2=1 mode and it should work... no 5 axis math required

 

Make some tests with L2=0 / L2=1 switches... I don't remember why but I went with L2=1... (I think it was something in Pro/NC)

 

Millplus are great controls... I'd love to work with them again... and once you add some logic to handle tool retraction between tool changes and milling modes you can trust blindly on these controls...

 

Hope that helps,

 

Daniel

[TK-32™]

G93 C=1 is awesome. Ive used it before. Thanks for your help guys. I think I'm going in tomorrow Sunday and try all this fun stuff

[crazy^millman]

Daniel was hoping to hear from my Brazilian friend. Hope all is well. Thanks for the sharing of that information it will help them go a long way. Awesome machine we got the machsim done for it and it is good for checking clearance and stuff.

 

Past 360 degree what are you crazy my friend anything over 10 degrees and you know I am lost. :whistle:

 

It is a whale of a job to sink you teeth into on the 1st 5 axis job, but TK has come along very well. He asks great questions lets me use his computer without getting upset and takes what I say and applies it. He is sorting is levels and drawing his fixtures in solids and making killer prints and set-up sheets. Give him a couple years and he will be teaching me stuff. So cool to see someone step into 5 axis land. It has been off and on about 3 months of my time on Saturday's but soon I will have taught him all I know and he will be on his on. I am glad to pass it on.

[Watcher]

BTW:

 

A very simple manner to find out if the post is doing transformation right now in Multiaxis is to see the XYZIJK coordinates in the NCI and compare them with the XYZ coordinates in the tape file. IJK are being computed as B and C so by looking at the XYZ you can have an idea if the PP is only missing G141 or if a new 5x logic needs to be implemented. It´s not a good idea to work in multiaxis mode in this control without G141... this function triggers many things in the machine dynamics and you will hate to have to re-post when your zero point changes after a probing operation or when your tool lenght is adjusted, or when you get mismatches in the surfaces because of variations in the pivot distance due to the load on the table (Maybe not in a DMU100T but certainly in a DMU70Evo)

 

Also, to have sucess with accurate features and GD&T (Specially true position) in DMGs it´s recommended to buy the 3D Quickset option to calibrate the pivot distances from time to time. It´s a DMG problem not seen in other brands, like Hermle for example...

 

Last but not least, the best Mastercam posts for these machines are IMHO from In-House, CIMCO and CAMAIX, not necessarily in this order. The good thing with CAMAIX is that besides the PP they also have an add-on to program probes for this control.

 

JM2C

 

HTH

 

Daniel

[Ron Branch @ 5th Axis]

Daniel, I was seeing some weird things so it should get taken care of this week. Work is piling up for them. They have a customer willing to dump a ton of work if they can get these parts cut so the owners are getting a little stressed to get it going.

 

Thanks for your insight and comments.

[TK-32™]

OK, so I re-read what Daniel wrote and guess what? It worked!!!!!

 

I used G7 L1=0 and G141

Here we go!!!!!!!!!!

 

Thank you guys very much for the help.

 

Here's a sample of the code that drove me nuts

 

 

%PM0001
( NOTES ) 
( N3710 )
( N3712 )
( N4252 )
( N4270 )
N1
N100 ( DATE -  27-06-12  TIME -  15:32 )
N110 ( 1/2 BULL EM .125 R   TOOL - 1  DIA. OFF. - 0  LEN. - 0  DIA. - .5 )
N120 G70
N130 G54 I1
N140 G74 Z-.1 L1
N150 G7 L1=1
N160 M11
N170 T1 M6
N180 M58
N190 G7 A5=0. B5=-83.035 C5=-45.171 L1=2
N200 G90
N210 G0 X1.673 Y.1994
N220 S10000 M3
N230 M10
N240 Z4.
N250 Z3.925
N260 G1 Z3.9 F200.
N270 X1.6743 Y.1997 Z3.886
( OPTI ROUGH TOOLPATH IN 3+2 )
N3670 X2.212 Y-1.224 Z2.2301
N3680 Z2.2757
N3690 G0 Z4.
N3700 ( CHECK )
N3710 G7 L1=0 <--- L1=0 "SHIFTS" THE PLANES WITHOUT MOVING THE MACHINE 
N3712 G141    <--- I GUESS THIS CODE ACTIVATES 5 AXIS
N3720 G0 X-2.6022 Y2.9007 Z2.1609 C-45.171 B-83.035
N3730 G1 X-2.966 Y2.5542 Z2.223 C-42.362 B-82.459 F120.
( 5AXIS CURVE TOOLPATH )
N4200 X.1697 Y-4.0108 Z2.6938 C74.829 B-83.035
N4210 G174
N4220 G40
N4230 M58
N4240 G7 A5=0. B5=-83.035 C5=74.829 L1=2
N4250 G90
( OPTI ROUGH TOOLPATH IN 3+2 ) 
N4252 Z4.     <---- I ADDED THIS Z VALUE HERE OTHERWISE SOFTWARE SWITCH LIMMIT TRIPS
N4260 G0 X1.673 Y.1994
N4270 Z4.     <----( THIS SHOULD BE BEFORE X,Y MOVES )   
N4280 Z3.925
N4290 G1 Z3.9 F200.
N4300 X1.6743 Y.1997 Z3.886
( OPTI ROUGH TOOLPATH IN 3+2 )
N7700 X2.212 Y-1.224 Z2.2301
N7710 Z2.2757
N7720 G0 Z4.
N7730 M5
N7740 G174
N7750 G74 Z-.1 L1
N7760 M56
N7770 G7
N7780 G74 X-0.1 Y-0.1
N7790 G74 B0
N7800 G27
N7810 G74 B0 C0
N7820 G93 C3=1
N7830 G90
N7840 M30

[TK-32™]

:thumbsup: :thumbsup:

[?Mark]

Watcher, Ron and TK, how do you like those machines? Pros/cons?

TK, what kind of material are you cutting?

We're looking into DMU vs Mori NMV.

 

TIA

[TK-32™]

Mark, this is a 2002 machine we got used about two years ago.

We recently had a ball screw replaced. But I think this machine has seen lots of hours.

This was our first multi axis machine so I can't really say much. Everythig else I have programmed before was fanuc so it took a little bit of time to get used to the codes. We cut mostly aluminum.

 

It's a German machine. Well built. I joke a lot about how even the coolant nozzle is an intricate artifact. It I got clogged one and when I took it apart I think I had like 15 different parts on the table.

The control is a Millplus IT controll.

[crazy^millman]

I think it is an awesome machine and after being around it for a while I have a whole new respect for these machines. If it were my shop they would get a serious consideration from me. The fact that the control from 2002 was doing what some controls can not even do today says a lot about the controls. Watcher (Daniel) has tons of experience with these machines. Also the dealers in Germany (Intercam) can give some good insight. When I was at EMO last year DMG/Mori had one whole building to themselves something like $40 million Euro to rent and I heard they sold every machine that went to the show at the show. The Germany mentality is different than the American mentality. Most place I worked it was get it done and worry about quality only if the customer complains. I was never that way and always called crazy because quality was the most important part of my job. Anyone can make parts, but quality good looking and everything right was always my concern. I held up 2000 parts one day going out the door, because they were not deburred to my standards. The owner was pissed me holding up an order, but he did not get the parts deburred to my standard and I sat there and starting deburring parts. After 45 minutes he seen I was serious and stopped the shop and we all sat there and deburred the parts to my standards. Huh seems off the subject, but it is all relative to the German thought process. There is almost no shop without a CMM there where I can remember working in and going to so many shops that didn't or care to even have one. Same thing with these machines the care and consideration put into them is a whole different thought process. I am not saying one is better than the other it is just different and where do you want to go with your work? Do you want to introduce a different type of control to the mix? What type of work are you doing will it's envelope? I like the C axis table and the B Tilt head. I like the Z table going up and done and keeping the heads mass limited to just the X and Y direction. Just look and evaluate and then go from there.

[crazy^millman]

TK that is great new so are you cutting the impellers yet?

[TK-32™]

I start today.

[Watcher]

Glad it worked for you! :thumbsup:

 

Out-of-curiosity: Millplus Controls were originally Philips 432 Controls... Dutch's stuff in fact... And it still being developed in The Nederlands... Eindhoven - City where Philips HQ is.

 

When Phillips decided to sold their CNC division to Heidenhain, the product turned into Millplus - From Heidenhain... and DMG kept the partnership started when they were only MAHO...

 

Google this: MAHO MH / PHILIPS 432 - There's a lot of history behind this subject...

 

Phillips 432/Millplus were so operator friendly and innovative back then that Heidenhain incorporated many of their features in their TNC product line... (TNC 426/430/530)

 

JM2C,

 

Daniel

[TK-32™]

UPDATE

 

Hello everyone, I had to leave this project for a little bit but I'm back at it. We are still working on the post.

 

In the mean time I edit by hand and make it run. Here's a video of the current state of affairs. As you guys can see, the program runs kind of choppy. Sometimes it stops as in Feed Hold but it shows "Running". the only way to get it going again is if I press Feed Hold button and then Cycle Start again. When it starts sometimes i can read the "REPOS"(repositioning) command on the control and then it goes.

I remember this before. I just can't remember if it was before or after we adjusted the kinematics on this machine. We all are hoping it's not the kinematics again.

Anyways, I hope you guys think this is as cool as we all here do.

 

9you gotta click on the video and it will re-direct you)

[crazy^millman]

That bring a tear to my eye. I feel like a proud Dad watching his son drive his first car.

 

Thanks TK-32. So I ain't all that crazy after all am I???

 

Try Turning down the programmed feed rate, or figure out how to active the look ahead that should take of the catch ups on the control.

[Watcher]

TK,

 

I suppose you have a Millplus V5.x control (Probably 5.2)

 

For the acceleration issues, look at the manual, search for G28 with I6 and I7 registers - I don't remember exactly but I think it helped me in Multiaxis, I remember I added support for it in our PP...

 

In roughing, you may increase the tolerances and acceleration factors and get a smoother move... V5.2 is MS-DOS based and it does not like 5 axis too much... V6 is better because it plays with faster hardware...

 

Using the same rule, you may want to use I6 and I7 with smaller values for highly precise surfaces... and DMG machines without their 3D Quick-Set optional may have some difficulties to hold tight dimensions in 5x (Including 3+2) because of their thermal instability and variations on the payload over the table... a head/table machine is less affected by this but the pivot point moves slightly depending on the temperature... If you don't have tight features to cut, you are good...

 

Millplus manuals can be found here

 

Perhaps a smaller acceleration even for roughing can help too... maybe a bigger tolerance in I7 and a smaller % in I6 can help... play with I6 and I7 until you find better results..

 

Man, I know how you are feeling now after overcoming the 5x initial challenges... good teacher you had eh - I was not that lucky!

 

Just kidding - Kudos to you and let me know if you need a Millplus programmer... - I love these controls and I have to admit I'm a bit jealous here!

 

Read these manuals whenever you can - I learned a lot with them and Millplus is one of the best documented controls out there yet it is unknown by many people...

 

Great video!

 

Cheers,

 

Daniel

[Jim at Gentex]

I'm also running a DMU with the MillPlus control which was purchased new in 2006.

Mine is the 80T which looks exactly like the machine in the video but I think a few inches smaller work envelope.

 

I haven't seen any of the new machines since DMG merged with Mori, but like Ron said, they couldn't sell them fast enough at the EMO show.

 

I enjoy programming and operating this machine every day and I always look forward to the challenging parts like the one in the video.

 

Yes, G141 enables 3D milling, and G40 cancels it.

I also noticed you are working in the M58 range.

That's cool, but if you ever need the full -120 degrees of B axis rotation, you change that to M59 and you get full range of travel on all 5 axes.

(Disclaimer: Use M59 with extreme caution!! )

 

If you can do that impeller job with your current post I would say that with the exception of a few tweaks, you are there.