What's new
What's new

Simultaneous 5 axis on Doosan/Fanuc with DWO, TCPC, WSEC etc

Andrew HSE

Plastic
Joined
Feb 8, 2021
Good afternoon,

I've been running Haas mills for ten years now, with our latest Haas being a UMC750SS. 6 months later we bought a Doosan DVF5000, a similar sized machine, but with a Fanuc 30i controller. It is nowhere near as user friendly as the Haas, but oh well, it's here now!

I'm having issues with regards to part location, work coordinates, tool lengths and feeds when using 5 axis simultaneous code generated by our CAM software OneCNC. I can configure the post to output the code required easy enough, I just don't know what that code is!

At this stage G54 is set to x0 y0 z-500ish as being the centre of the table, and the part location offset from the position is stored in G54.2p1
First point of frustration is that the Doosan GUI wont store the part location in G54.2p1, it has to be manually entered which leads to potential errors. If anyone has any advice on this, preferably without running MDI programs or macros that would be amazing. Doosan seems to show no interest.

With the above setup for 3+2 machining I am using G54, G54.2p1, and G43 and seem to have success, though it seems more complex than the Haas and its ability to set a single G54 with the probing cycles. All programs are created with OneCNC, and the work origin is in the logical positionfor each part. I don't want to have to stuff around with applying offsets for the CAM to output modified code to suit the position of the part in the machine.

Using the same G54, G54.2p1, and G43 codes the simultaneous machining works fine providing the part is centred on the table in X and Y. Any offset in x or y results in funny looking parts, but at a glance it appears to be doing the correct thing as a straight C axis rotate move with the table tilted at 45 degrees forces the cutter to move in X, Y , Z, and C as though its following the offset correctly. Its clearly not right though. The feedrate isn't correct either, though I was lead to believe that when in G94 the Fanuc control would adjust the speed to keep the mm/min constant.

I get lost when it comes to choosing between TCPC, DWO, WSEC, and where and when to use G43.4 vs G4 etc.

The below link is a iPhone video of the current part, showing the toolpath and the way the feed is inconsistent.

Link

And here is what I have generated at the start of a program currently
%
O0001
G21 G40 G80 G90 G49 G69 G54.2P0
G53 Z0
G0 X0 Y0 B0 C0
T7 M06 (8MM END MILL)
G00 G90 S3000 M03
G54
G54.2P1
G43 H7 (X115.18 Y0.988)
M11 (unlock 4)
M39 (unlock 5)
G00 X115.18 Y0.988 B45. C180.
Z100.
Z27.317
G01 Z25.11 F250.
X115.092 Y0.985
And then the following is the feed moves around the part

If anyone can give me any information that would be great!

Also, for reference here is my Haas code in all its simplicity
G00 G40 G49 G80
G00 G90 G54
G00 G53 Z0
G00 G53 X-750.146 Y-213.129 (tool change position)
G255
G90 G00 G54 B0 C0
T7 M06 (8MM END MILL)
G90 G80 G40
S3000 M03
G43 H7
G255
M11
M13
G93
G234 H7
G00 X-152.155 Y-0.988 Z-10.734 B45. C180.
X-100.76 Y-0.988 Z-62.128
 
You need to call Doosan and start yelling.

A Fanuc control is a general purpose thing that they sell to any MTB and can be configured a million ways under the sun. Haas has the advantage of being one company, with one programming manual, and one control. It is on Doosan Australia to set you up for success by helping you dial in your programming style and helping you work with your CAM maker to get a working post processor. This is why Apps Engineers exist...

Looking at your code; Haas is using both Dynamic Work Offsets (G254) and Tool Center Point Control (G234). The Doosan code is only using Rotary Work Offsets (G54.2) which are really intended for 4 axis machines in indexing applications, while the tool comp is bog standard G43 height compensation. What I think you are intending is to be using Workpiece Setting Error Comp (G54.4) which is analogous to Haas Dynamic Work Offsets, and you're absolutely intending to use Tool Center Point Control (G43.4).

How you set that up on a Doosan and call it in your programs is beyond my pay-grade, and it is on Doosan to help you walk through that, with the added caveat that it is also on OneCNC to give you a post that jives with how Doosan configured the Fanuc to do all of this (mind you, Fanuc has configuration options that make the machine perform dramatically differently with these technologies, depending on how the parameter are set... hence Doosan needs to give OneCNC guidance for the post development).

If Doosan continues to show "no interest" in helping a customer get their massive capital asset functioning as intended, you need to start showing interest in getting them to take back the god damn machine.
 
Did you have a post written for the machine? I ran a UMC750 years ago, we had postability write a post and machine sim for it. No problems for the most part, output correct codes for DWO and TCPC. I would start at the posting level and make sure that is correct. It will cost money (unless Doosan provides that with machine?). I was using MCX 8 and 9 with ours...
 
You're not utilizing the GUI correctly. There is a function to access extended work coordinates like G54.1P1 etc. Look at the bottom of the display for "Advanced" and PRESS IT.
I used to do training and applications for Doosan.
Also, there's some five access training materials. Contact LockNut (Paul) here on PM. I used to work with him. Great five ax guy. Tell him I sent you.
 
OK, I ride in on my guilded steed. First, the DVF5000 is not programmed from the center of rotation and this should not go into a work offset (G54). The center of rotation is stored in the kinematics parameters. You set a work offset just like any part on a 3 axis mill. The control does the rest when you use either TCP (G43.4) or TWP (G68.2). At this point, there is no need for DWO either. If your kinematics are dialed in, and the factory settings will be as good as they get right now, then TCP and TWP will give you great results.

And Douglas is right, you are not using the GUI properly. Your dealer should have gone over this with you already. Contact them.

Sounds like you need a lot of training, beyond just the machine. Nobody should be expected to jump into 5 axis not knowing what the machine is supposed to do or how your code should look. Get the required training from your dealer.

I have one document that I consider my bible for this machine, PM me your email address and I will send it to you. read it all, there is some great info in it and it will answer most of your questions.

regards,
Paul Anderson
Applications Engineer
Doosan Machine Tools America
[email protected]
 
You need to call Doosan and start yelling.

A Fanuc control is a general purpose thing that they sell to any MTB and can be configured a million ways under the sun. Haas has the advantage of being one company, with one programming manual, and one control. It is on Doosan Australia to set you up for success by helping you dial in your programming style and helping you work with your CAM maker to get a working post processor. This is why Apps Engineers exist...

Looking at your code; Haas is using both Dynamic Work Offsets (G254) and Tool Center Point Control (G234). The Doosan code is only using Rotary Work Offsets (G54.2) which are really intended for 4 axis machines in indexing applications, while the tool comp is bog standard G43 height compensation. What I think you are intending is to be using Workpiece Setting Error Comp (G54.4) which is analogous to Haas Dynamic Work Offsets, and you're absolutely intending to use Tool Center Point Control (G43.4).

How you set that up on a Doosan and call it in your programs is beyond my pay-grade, and it is on Doosan to help you walk through that, with the added caveat that it is also on OneCNC to give you a post that jives with how Doosan configured the Fanuc to do all of this (mind you, Fanuc has configuration options that make the machine perform dramatically differently with these technologies, depending on how the parameter are set... hence Doosan needs to give OneCNC guidance for the post development).

If Doosan continues to show "no interest" in helping a customer get their massive capital asset functioning as intended, you need to start showing interest in getting them to take back the god damn machine.


GKoenig, where did you get the idea that Doosan wasn't listening. The OP made no mention of not getting assistance from Doosan Australia and made no mention of Doosan not showing "interest". Don't you think it's a little soon to "start showing interest in getting them to take back the god damn machine."
My, aren't we jumpy this morning. Go have another cup of coffee.

Paul
 
OK, I ride in on my guilded steed. :D

And Douglas is right, you are not using the GUI properly. Your dealer should have gone over this with you already. Contact them.


I have one document that I consider my bible for this machine, PM me your email address and I will send it to you. read it all, there is some great info in it and it will answer most of your questions.

I can vouch for this information. A must have!
 
GKoenig, where did you get the idea that Doosan wasn't listening. The OP made no mention of not getting assistance from Doosan Australia and made no mention of Doosan not showing "interest". Don't you think it's a little soon to "start showing interest in getting them to take back the god damn machine."
My, aren't we jumpy this morning. Go have another cup of coffee.

Paul

Doosan seems to show no interest.

You missed that part?
 
You need to call Doosan and start yelling.


If Doosan continues to show "no interest" in helping a customer get their massive capital asset functioning as intended, you need to start showing interest in getting them to take back the god damn machine.

First off, before "yelling" you should advise to start talking. Calmly. Like an adult.
Secondly, as someone who ran training for Doosan for years, and was a A/E as well, I can assure that Doosan is VERY interested in a customer getting his machine running properly.

While I no longer work there, I take aburaage that you are making as tho Doosan doesn't care about its customers. They do care and they want to see their customers succeed. I should know, I trained many of their staff, and even the ones I didn't train, I know, beyond all doubt, that they are more than capable of helping.

Lastly, the Fanuc CNC on the DVF is anything but generic. It's well optioned and well equipped for the task. Again, speaking from experience as I ran/setup/programmed DVF's during my tenure there.
 
First off, before "yelling" you should advise to start talking. Calmly. Like an adult.
Secondly, as someone who ran training for Doosan for years, and was a A/E as well, I can assure that Doosan is VERY interested in a customer getting his machine running properly.

While I no longer work there, I take aburaage that you are making as tho Doosan doesn't care about its customers. They do care and they want to see their customers succeed. I should know, I trained many of their staff, and even the ones I didn't train, I know, beyond all doubt, that they are more than capable of helping.

Lastly, the Fanuc CNC on the DVF is anything but generic. It's well optioned and well equipped for the task. Again, speaking from experience as I ran/setup/programmed DVF's during my tenure there.

Instead of being so anxious to jump to the defence of your former employer, you should at least entertain the possibility that whoever sold the machine to OP's employers were not as conscientious as the people that you worked with.

It's absolutely plain to see that they have not provided adequate training.
 
Instead of being so anxious to jump to the defence of your former employer, you should at least entertain the possibility that whoever sold the machine to OP's employers were not as conscientious as the people that you worked with.

It's absolutely plain to see that they have not provided adequate training.


How do you know this based on a new member with but a single post? You may be correct but you don't know that. Maybe they haven't received training yet and he is plowing ahead trying to figure things out. I can't speak for our brothers in Australia but I know in the US we provide pretty good training. Doosan Australia is a whole different company than Doosan America.

Quote=You missed that part?
Yes, I missed that part. Do you know how many times I have heard that because a customer didn't simply hear what they wanted?
There is a very specific method to running this machine based on the options provided. Industry standard today and quite different than 20 years ago.
 
How do you know this based on a new member with but a single post? You may be correct but you don't know that. Maybe they haven't received training yet and he is plowing ahead trying to figure things out. I can't speak for our brothers in Australia but I know in the US we provide pretty good training. Doosan Australia is a whole different company than Doosan America.

Quote=You missed that part?
Yes, I missed that part. Do you know how many times I have heard that because a customer didn't simply hear what they wanted?
There is a very specific method to running this machine based on the options provided. Industry standard today and quite different than 20 years ago.

I have no reason to believe I'm right.

Simply that here in the UK Doosan are sold and supported by a third party, and it's likely that it's the same in Australia, and third party machine sellers are all over the place in terms of how they treat their customers.

Unless you know those people personally, you shouldn't be so quick to assume that they are treating the OP as well as you and your colleagues do.
 
I have no reason to believe I'm right.

Simply that here in the UK Doosan are sold and supported by a third party, and it's likely that it's the same in Australia, and third party machine sellers are all over the place in terms of how they treat their customers.

Unless you know those people personally, you shouldn't be so quick to assume that they are treating the OP as well as you and your colleagues do.

Doosan has representation in Australia. It's just too easy to say "send it back" when in fact a little training and some research can go a long way.
 
You need to call Doosan and start yelling.

A Fanuc control is a general purpose thing that they sell to any MTB and can be configured a million ways under the sun. Haas has the advantage of being one company, with one programming manual, and one control. It is on Doosan Australia to set you up for success by helping you dial in your programming style and helping you work with your CAM maker to get a working post processor. This is why Apps Engineers exist...

Looking at your code; Haas is using both Dynamic Work Offsets (G254) and Tool Center Point Control (G234). The Doosan code is only using Rotary Work Offsets (G54.2) which are really intended for 4 axis machines in indexing applications, while the tool comp is bog standard G43 height compensation. What I think you are intending is to be using Workpiece Setting Error Comp (G54.4) which is analogous to Haas Dynamic Work Offsets, and you're absolutely intending to use Tool Center Point Control (G43.4).

How you set that up on a Doosan and call it in your programs is beyond my pay-grade, and it is on Doosan to help you walk through that, with the added caveat that it is also on OneCNC to give you a post that jives with how Doosan configured the Fanuc to do all of this (mind you, Fanuc has configuration options that make the machine perform dramatically differently with these technologies, depending on how the parameter are set... hence Doosan needs to give OneCNC guidance for the post development).

If Doosan continues to show "no interest" in helping a customer get their massive capital asset functioning as intended, you need to start showing interest in getting them to take back the god damn machine.

pretty much what gkoenig said. your G54 should be located on the part, not center of rotation, thats the whole point of using dynamic work offsets and tool centerpoint control.
so for one, your post isnt configured correctly for either dynamic work offsets or TCPC. that wont be on doosan, you'll need to reach out to OneCNC or whoever creates your posts.
i honestly dont see how this is on doosan, you have the manual that explains what the post needs to contain, i'm sure they CAN help you, but going as far as making them take the machine back because he doesnt have the right post is a bit much IMO.
 
pretty much what gkoenig said. your G54 should be located on the part, not center of rotation, thats the whole point of using dynamic work offsets and tool centerpoint control.
so for one, your post isnt configured correctly for either dynamic work offsets or TCPC. that wont be on doosan, you'll need to reach out to OneCNC or whoever creates your posts.
i honestly dont see how this is on doosan, you have the manual that explains what the post needs to contain, i'm sure they CAN help you, but going as far as making them take the machine back because he doesnt have the right post is a bit much IMO.

What's on Doosan('s affiliate agency) is that OP doesn't know how to use his machine, he has clearly received completely inadequate training.

From the OP:

...I can configure the post to output the code required easy enough, I just don't know what that code is!

As devil's advocate, it's obviously possible that OP's employers ordered a new 5ax mill from an unfamiliar mtb, with an unfamiliar control, and elected NOT to include basic training in the purchase.

Likely? I don't think so.
 
What's on Doosan('s affiliate agency) is that OP doesn't know how to use his machine, he has clearly received completely inadequate training.

From the OP:



As devil's advocate, it's obviously possible that OP's employers ordered a new 5ax mill from an unfamiliar mtb, with an unfamiliar control, and elected NOT to include basic training in the purchase.

Likely? I don't think so.

I am not so sure. I didn't get any Haas training on the UMC750 I ran. Other than basic, basic stuff, but certainly nothing about how code should look, or if I (my cam) was using DWO or TCPC correctly. That was mostly all on our post developer we paid to get a good post that utilized the 5 axis stuff properly, and even then I had to figure out alot of the programming on my own.

edit: and it could be they elected to not get any training. We bought NX and were told to figure it out. Begged for months to even get a basic class on it after fumbling around with it.
 
I am not so sure. I didn't get any Haas training on the UMC750 I ran. Other than basic, basic stuff, but certainly nothing about how code should look, or if I (my cam) was using DWO or TCPC correctly. That was mostly all on our post developer we paid to get a good post that utilized the 5 axis stuff properly, and even then I had to figure out alot of the programming on my own.

edit: and it could be they elected to not get any training. We bought NX and were told to figure it out. Begged for months to even get a basic class on it after fumbling around with it.

mmmhm...
ASSuming is never a good strategy, lol.
 
I am not so sure. I didn't get any Haas training on the UMC750 I ran. Other than basic, basic stuff, but certainly nothing about how code should look, or if I (my cam) was using DWO or TCPC correctly. That was mostly all on our post developer we paid to get a good post that utilized the 5 axis stuff properly, and even then I had to figure out alot of the programming on my own.

edit: and it could be they elected to not get any training. We bought NX and were told to figure it out. Begged for months to even get a basic class on it after fumbling around with it.

Well, that's the polar opposite to my experience buying a 5ax machine...
 
G68.2 is magic. You don't have to worry about where your vise is on the table or whatever, just probe your WCS in and start cutting.

Lots of parameter stuff to dig into with a FANUC in 5-axis so if you see oddball or jerky rapid moves during repositioning moves and such there is usually a way to smooth things out.

One time you can get in trouble with TWP (Transform Work Plane, G68.2) is if you need to pick up a feature on an angle. You need to do the math for the offset and then program off that point in CAM (or with a program like CAMplete Truepath you can do the work right in the software using measure and transform functions).

Hope you get it figured.
 








 
Back
Top