Doosan DVF 8000 Verify/Post issue?

[Bill Henderson]

We recently purchased this machine new. First parts run on it had issues in tool offsets using dynamic. Post was verified and it ended up being some parameters or interpretation software error. Thought it was fixed and finally made a good part.

Now my parts are on this machine and an off-site programmer made the programs. The verify in simulation looks correct in 5X swarf etc... but in reality my part is scrapped.  Wall thickness which is supposed to be the same at various points is very narrow.

G59 G17 G90
A-90. C180.
G68.2 X0. Y0. Z0. I-180. J-90. K0.
G53.1
G94
G05.1 Q1 R5.

My question would be ... could the tool vector be calculated wrong at the machine? The code looks correct and simulates correctly.

Seeing the tool offsets were being calculated incorrectly before and it took Doosan reps 10 days to figure it out, I am wondering if it's just the machine again.

 

BTW He programmed the pieces to center of rotation.

 

I haven't been on here in years mainly due to the fact I rarely if ever have to program anymore.

 

Thank you for any insight.

[gcode]

Our 5X gantry mill with a Fanuc 31 would look like this for a full 5x swarf toolpath

T3 M06 (1" X .19R SANDVIK INSERT MILL)
G54 G17 G90
G00 A-4.3 B.755
X-3.4265 Y15.412
G01 G94 X-3.4265 Y15.412 S1528 M03 F200.
G43.4 H3 X-3.4265 Y15.412 Z3. M08
Z2.5197

 

The sample you posted would be a tilted tool plane 3+ 2 toolpath

[gcode]

Note... some really good posts use tilted tool plane output to position the tool first,

then switch to G43.4 for the full 5X toolpath

[cncappsjames]

Personally, I steer clear of programming 5-Axis machines using the Center of Rotation as the work offset. That just invites troubleshooting problems.

More than likely Bill, one or more of your #19700-#19705 parameters are off.

#19700 = COR X

#19701 = COR Y

#19702 = COR Z

#19703 = 1/2 Offset X - Rotary Table Position deviation from COR X (N/A on A/C Machines)

#19704 = 1/2 Offset Y - Rotary Table Position deviation from COR Y (N/A on B/C Machines)

#19705 = 1/2 Offset Z - dist. from COR Z to top of the pallet (N/A on A/B Machines)

[Colin Gilchrist]

36 minutes ago, cncappsjames said:

Personally, I steer clear of programming 5-Axis machines using the Center of Rotation as the work offset. That just invites troubleshooting problems.

More than likely Bill, one or more of your #19700-#19705 parameters are off.

#19700 = COR X

#19701 = COR Y

#19702 = COR Z

#19703 = 1/2 Offset X - Rotary Table Position deviation from COR X (N/A on A/C Machines)

#19704 = 1/2 Offset Y - Rotary Table Position deviation from COR Y (N/A on B/C Machines)

#19705 = 1/2 Offset Z - dist. from COR Z to top of the pallet (N/A on A/B Machines)

So often, this is the exact problem.

For Dynamic Codes to work, you must have:

• Calibrated Tool Measurements
• Calibrated Part measurements
• Calibrated Center-of-Rotation Parameters.
• Correctly formatted NC Code, that references that correctly calibrated data. 

[PAnderson]

On 8/4/2021 at 2:18 PM, cncappsjames said:

Personally, I steer clear of programming 5-Axis machines using the Center of Rotation as the work offset. That just invites troubleshooting problems.

More than likely Bill, one or more of your #19700-#19705 parameters are off.

#19700 = COR X    Should be "0"

#19701 = COR Y    Should be "0" give or take a few microns ideally

#19702 = COR Z    Should be -740.00 give or take a .01MM

#19703 = 1/2 Offset X - Rotary Table Position deviation from COR X (N/A on A/C Machines)   Should be "0"

#19704 = 1/2 Offset Y - Rotary Table Position deviation from COR Y (N/A on B/C Machines)  Should be "0" give or take a few microns.

#19705 = 1/2 Offset Z - dist. from COR Z to top of the pallet (N/A on A/B Machines)    Should be -100.00 give or take a few microns.

If indeed this was programmed from the center of rotation, then the 19700-19705 parameters would not play a role at all. In TCP they certainly would. These values would be in the post processor. #19702 and #19705 would need to be exact. With TCP, #19705 is not used. It would be used when programming from the COR and MUST be exact.

The kinematics parameters would indeed affect G68.2 if that is all that was used. Could you post more of the code? I have all of my posts to use G68.2 to position the tool safely over the part after A and C rotation, turn it off and straight to G43.4. Almost always, I suggest NOT updating the kinematics right after install because the values from the factory are the best during machine build. I ask customers to run the machine with their first parts until errors are seen, then take a look at what is going on.

Was the machine lasered during installation? Is it bolted to the floor?

I'm in 5 axis applications with Doosan. Call me if you have questions. 973-618-2457 I may have already been involved with this machine through Adams.

Here are the values from a recent machine, newly installed.

N19700Q1L1P0.0L2P0.0
N19701Q1L1P-0.012L2P0.0
N19702Q1L1P-739.932L2P0.0
N19703Q1L1P0.0L2P0.0
N19704Q1L1P0.012L2P0.0
N19705Q1L1P-100.068L2P0.0

[Bill Henderson]

 I don't have the code any longer. They re-wrote the program for indexed surface milling. These are one off inconel parts for R & D. 

You may have been here when the machine was first checked after issues. Yes it is bolted to a newly poured floor.

 

Thanks James. Haven't heard from you since you left FB. Hope all is well. 

Tom thank you as well. Been a long time.

 

Hopefully we will be able to use the machine to it's full capability but right now I have hardware that absolutely NEEDS to ship.

[cncappsjames]

3 hours ago, Bill Henderson said:

Thanks James. Haven't heard from you since you left FB. Hope all is well.

I left FB October 2020 @12:01am. No fanfare. Just killed the account completely. It was pretty funny, I must've gotten a dozen e-mails from FB for the next month to reinstate my account and nothing would be lost. LOL

I'm good. Traveling a little more than usual, but it's good. I've always like to travel for business. I hope you are well also.

4 hours ago, PAnderson said:

If indeed this was programmed from the center of rotation, then the 19700-19705 parameters would not play a role at all.

It would depend. We have  a customer that actually takes their #19700-#19705 numbers converts them to inch then puts those numbers in their Work Offset. I only have maybe 2 customers that do that but they chase work offsets all the time. I warned against it.

That said, if no 5-Axis functions are used (G54.4, G68.2, or G43.4) then you are correct, those parameters have no bearing on anything since the functions using those parameters are not invoked.

[cncappsjames]

4 hours ago, PAnderson said:

N19700Q1L1P0.0L2P0.0

N19701Q1L1P-0.012L2P0.0
N19702Q1L1P-739.932L2P0.0
N19703Q1L1P0.0L2P0.0
N19704Q1L1P0.012L2P0.0
N19705Q1L1P-100.068L2P0.0

Those are your machine kinematics?

[Leon82]

2 hours ago, cncappsjames said:

Those are your machine kinematics?

It's certainly possible.  Our yasdas are like that. Machine zero of the center in x and y but it zero returns to the positive side at the end of travel

[cncappsjames]

That #19705 tho...