Mastercam 2022 5 axis Drilling

[Dave_WDM]

Slowly working my way into 5 axis simultaneous. Machine is a UMC500
Running the Caminstructor 5 axis - lesson 2. Can provide program.
So I roughed with optirough, and finished with multiaxis flow. Everything worked as it should.

I went to drill the holes, and usually when I drill holes I'll create a new plane as required. But Caminstructor had me use 5 axis drilling. Seemed a lot quicker as setting up separate planes is not required Control click and let er rip. HOWEVER, it crashed my machine. Not hard, material was just aluminum and I stopped her pretty quick. It seems that TCPC never activated. So the question is, did I miss a step when doing the drill parameters in Mastercam, or do I have a bad post for the machine? It tried to post using DWO, didnt compensate when the axis moved, broke the drill and tried to plunge into the part ~2 inches or so.

Thanks for any insight.

 

[D Nelson]

Check your program and see if it added a g55 on you. We’re you using g54?
Don


Sent from my iPhone using Tapatalk Pro

 

[Dave_WDM]

Yeah using G54. I dont have the code on me, can check monday. If I remember right, when I was doing the flow toolpath, it calls the tool, activates G254 DWO, then cancels it with G255, then activates G234? Maybe the wrong number to activate TCPC
But when I did the 5 axis drill path, it calls the tool then activates G254 and thats at. Drilled the first 20 or so holes correctly, as soon as it rotated the B axis, broke the drill, and it plunged into the part. So my main concern is, did i miss program in Mastercam, is there something I did on my end that caused this. Or is there something wrong with the post. Because like I said, I've done 3+2 and dabbled in some simultaneous toolpaths and they've worked correctly. So I am confused as to why it crashed this time.

 

[rcoope]

Does it look OK in the simulator? Interesting about calling both DWO and TCPC in the same program. There doesn't seem to be a way to cancel TCPC. I'd experiment with doing the same holes separately and see if not invoking TCPC first makes a difference.

Hey while I'm here how is the Caminstructor series and do you have any idea how it compares to MasterCAM University? I've done the latter for lathe successfully but we need to get some more 5 axis instruction going.

 

[Dave_WDM]

Does it look OK in the simulator? Interesting about calling both DWO and TCPC in the same program. There doesn't seem to be a way to cancel TCPC. I'd experiment with doing the same holes separately and see if not invoking TCPC first makes a difference.

Hey while I'm here how is the Caminstructor series and do you have any idea how it compares to MasterCAM University? I've done the latter for lathe successfully but we need to get some more 5 axis instruction going.

Yes, everything simulates and verifies and backplots correctly. Which is why im pretty confused as to why it happened. I always model my toolholder and workholding so I know where everything is at. I picked up on 3+2 pretty quick, but this simultaneous is a whole new ballgame. As for TCPC, I never enabled/disabled it to my knowledge. I've just been running the code as the post spits it out.

Im just diving into the 5 axis portion. They have like 8 lessons with a PDF and a video to go along with it. Click this box, change this value to xyz, etc. The thing I don't like is they dont go super in depth on what each option does. So sometimes I feel like Im just plugging and chugging without understanding how everything actually works and thats the frustrating part. Theres a ton of new options and features in the 5 axis toolpaths, but I don't know what 90% of them actually do.

 

[TKassoc]

Check the code. My post for 5-axis drilling got broken moving to 2022. It would simulate fine but the posted code ignored the drill retract plane and moved between holes without getting the drill back out of the hole.

 

[Dave_WDM]

Check the code. My post for 5-axis drilling got broken moving to 2022. It would simulate fine but the posted code ignored the drill retract plane and moved between holes without getting the drill back out of the hole.

Okay I'll definitely look into it. We were videoing since it was the first time we were doing anything besides 3+2 and that sounds pretty similar. Ours retracts out of the hole, but never picks up any sort of clearance of TCPC. So when the B axis rotated, it snapped the drill, and plunged into the part.

 

[rcoope]

Yes, everything simulates and verifies and backplots correctly. Which is why im pretty confused as to why it happened. I always model my toolholder and workholding so I know where everything is at. I picked up on 3+2 pretty quick, but this simultaneous is a whole new ballgame. As for TCPC, I never enabled/disabled it to my knowledge. I've just been running the code as the post spits it out.

Im just diving into the 5 axis portion. They have like 8 lessons with a PDF and a video to go along with it. Click this box, change this value to xyz, etc. The thing I don't like is they dont go super in depth on what each option does. So sometimes I feel like Im just plugging and chugging without understanding how everything actually works and thats the frustrating part. Theres a ton of new options and features in the 5 axis toolpaths, but I don't know what 90% of them actually do.

We are trying to be clever with separate four and five axis machine definitions using our TRT-160 where the 5 axis version has DWO off but TCPC on. Then for the forth, with the tilt axis at 90 degrees the idea is to have DWO on. The 5th works but we haven't sorted out the 4th version. But I'm realizing in reading your post that this may be more complicated and you need DWO for certain 3+2 operations you might run in the same program as simultaneous 5 axis. The larger challenge here is related to what you said about the courses, and that's true of MCam U as well. MasterCAM with its legacy features and multiple ways to do things needs explanation of the intention of functions, in many cases how they overlap each other, and a bit of explanation of the overall architecture. Sounds like it will continue to be a mix of courses, and trying stuff, and sharing knowledge here!

 

[empower]

Yes, everything simulates and verifies and backplots correctly. Which is why im pretty confused as to why it happened. I always model my toolholder and workholding so I know where everything is at. I picked up on 3+2 pretty quick, but this simultaneous is a whole new ballgame. As for TCPC, I never enabled/disabled it to my knowledge. I've just been running the code as the post spits it out.

Im just diving into the 5 axis portion. They have like 8 lessons with a PDF and a video to go along with it. Click this box, change this value to xyz, etc. The thing I don't like is they dont go super in depth on what each option does. So sometimes I feel like Im just plugging and chugging without understanding how everything actually works and thats the frustrating part. Theres a ton of new options and features in the 5 axis toolpaths, but I don't know what 90% of them actually do.

most 'instructions' are usually like that. i've yet to see anyone explain what each function does, only like you said: change XYZ, blah blah blah...
worthless

 

[thesidetalker]

We are trying to be clever with separate four and five axis machine definitions using our TRT-160 where the 5 axis version has DWO off but TCPC on. Then for the forth, with the tilt axis at 90 degrees the idea is to have DWO on. The 5th works but we haven't sorted out the 4th version. But I'm realizing in reading your post that this may be more complicated and you need DWO for certain 3+2 operations you might run in the same program as simultaneous 5 axis.

Why are you thinking to have different machine definitions for one machine? What purpose would that serve to have only one, either DWO or TCPC available? It seems like it would be limiting down the road, or adding additional complications.
Esp on your "5 axis version" with DWO off, only TCPC on. You do know in TCPC you're only doing G0/G1 moves? No G2/3 arcs, no canned cycles, or 2D cutter comp G41/42

 

[rcoope]

SideTalker you're completely right about the DWO/TCPC here and as I've leaned in this thread, I'm wrong, but that's why we're here, to learn, and we'll fix that for both 4th and 5th axis set ups. There's a lot of trouble shooting history with our VAR editing our post and as is the case with a lot of stuff around here, we're all wondering why no one, including the course providers, VARs or machine vendors can give us good answers to what seem like questions that lots of people have.

The reason to have different machine definitions is you can generate simpler g-code. Our 4th axis concept is to turn the TRT-160's tilt axis, which in our case, is aligned with Y, to 90 so the platter is facing along the X-axis of the table and then use the platter as a 4th. The TRT-160 has a 1.6" bore in the platter so you can machine tube ends and everything but obviously if you're doing that you really really don't want to have the B axis inadvertently move. So might would ideally like to generate g-code with no B values at all so you can be assured the B never changes. Likewise with the three axis machine definition with the trunnion not being used you can generate g-code with no B or C values being posted at all. At least these things make the g-code easier to interpret.

Sorry Dave_WDM for derailing this thread (but I think somehow all these issues are coupled)!

 

[mike_w]

Im just diving into the 5 axis portion. They have like 8 lessons with a PDF and a video to go along with it. Click this box, change this value to xyz, etc. The thing I don't like is they dont go super in depth on what each option does. So sometimes I feel like Im just plugging and chugging without understanding how everything actually works and thats the frustrating part. Theres a ton of new options and features in the 5 axis toolpaths, but I don't know what 90% of them actually do.

most 'instructions' are usually like that. i've yet to see anyone explain what each function does, only like you said: change XYZ, blah blah blah...
worthless

The PDF's yes, it's hard to get fully in depth in explaining things, the books are already 500-600+ pages (we need to keep that in mind as these do get printed). Check the videos for more in depth explanation. No trees can be harmed due to the length of the videos. I take pride in not doing the 'put this value here and carry on' type training.

The issues you are seeing, your gcode should replicate what you see on screen. My fist check would be with the post and ensuring the required misc values are used to generate the needed DWO/TCPC. You post developer should have provided documentation on this. Without seeing a file I won't hazard to guess further.

Since we're here, what post are you using? What Mastercam version? What camInstructor lesson version?

 

[thesidetalker]

Our 4th axis concept is to turn the TRT-160's tilt axis, which in our case, is aligned with Y, to 90 so the platter is facing along the X-axis of the table and then use the platter as a 4th. The TRT-160 has a 1.6" bore in the platter so you can machine tube ends and everything but obviously if you're doing that you really really don't want to have the B axis inadvertently move. So might would ideally like to generate g-code with no B values at all so you can be assured the B never changes.

Ah, gotchya. In that case it makes sense...

Just watch out of that HomeG28 button! That could cause some headaches. Unless you can disable the tilt axis in machine setup? Never tried that myself.



I assume 5-axis drilling is also making swoopy [TCPC] linking moves to move from one location to another? Along with making it easier to select different holes without creating additional views or planes?

Funny, Surfcam has "5-axis drilling" which is only the second part of that equation. Even though it displays nice linking moves on the screen, it doesn't create any linking geometry which you can actually use by your post to generate those moves. It is simply hole locations at those different angles. One of these days I'll get around to trying my mastercam seat or something else. Seems there's never any time these days.


Post that code when you can, Dave

 

[LockNut]

I do 5 axis drilling a lot on a Fanuc control. It works great. Except that it cannot use TCP because TCP doesn't support canned cucles. Mine uses Tilted Working Plane and outputs a different G68.2 for each hole after returning Z Axis to home.

%
O0000 (CAVITY FOR TRIAL)
(POSTABILITY DOOSAN DVF 5000)
(MACHINE GROUP-1)
(MASTERCAM - 2022)
(T3 - 0.111 34 JOBBER DRILL - H3 - D3 - D0.1110")
G00 G17 G20 G40 G80 G90
G91 G28 Z0.
G90 B0. C0.
N3
(OPERATION NO - 5)
(OPERATION TYPE - PECK DRILL)
T3 M06(0.111 34 JOBBER DRILL)
G54 G17 G90
G00 B13.775 C120.
G68.2 X0. Y0. Z0. I-330. J-13.775 K330.719
G53.1
S10324 M03
X1.1727 Y-2.0913
G43 H3 Z1.6487
G94
G98 G83 Z-1.3512 R-.9763 Q.1 F51.62
G80
G49
G69
G91 G28 Z0.
G54 G90
B13.775 C105.
G68.2 X0. Y0. Z0. I-345. J-13.775 K330.719
G53.1
X1.1727 Y-2.0914
G43 H3 Z1.6487
G98 G83 X1.1727 Y-2.0914 Z-1.3512 R-.9763 Q.1 F51.62
G80
Z1.6487
G49
G69
G91 G28 Z0.
G54 G90
B13.775 C90.
G68.2 X0. Y0. Z0. I0. J-13.775 K330.719
G53.1
X1.1727 Y-2.0913
G43 H3 Z1.6487
G98 G83 X1.1727 Y-2.0913 Z-1.3512 R-.9763 Q.1 F51.62
G80
Z1.6487
G49
M05
G69
G91 G28 Z0.
G30 X0. Y0.
G90 B0. C0.
M30
%

 

[thesidetalker]

I do 5 axis drilling a lot on a Fanuc control. It works great. Except that it cannot use TCP because TCP doesn't support canned cucles. Mine uses Tilted Working Plane and outputs a different G68.2 for each hole after returning Z Axis to home.

Right. I use TWP and canned cycles too, but sometimes switch to TCP to link between holes. But one could also leave TCP on always and post out cycles long-hand.

My links are just one line to the next position, though. No swoopy moves flying around the part.

 

[Mtndew]

HOWEVER, it crashed my machine.

You don't use single block and distance to go?

did I miss a step when doing the drill parameters in Mastercam, or do I have a bad post for the machine?

Not sure if you missed a step (I'd have to see the file), having a bad post is unlikely since you've already been using it for 5 axis stuff.

5axis drilling is pretty simple and straightforward, but it's very easy to not have everything set right.

The one thing I will tell you to watch out for, is that after picking your geometry and then selecting 5 axis, go back and look at the geometry again to make sure it's pointing in the correct direction. I've noticed many times that it likes to flip the vectors on me after telling it that it's a 5 axis path.

I think this is noted on the official forums and will be fixed in the next update or version.

 

[Dave_WDM]

Okay here is the code:

G00 G17 G40 G80 G90 G93
(.283 TSC DRILL|TOOL - 13|DIA. OFF. - 13|LEN. - 13| DIA. - .28346457)
G53 Z0.
G53 Y0.
B0.
G53 X-23.
M11
M13
T13 M06
T10
G90 G54 C180. B90.
S9750 M03
M10
M12
G254 X3.149 Y-1.5
G43 H13 Z3.2
G94
G81 G99 Z2.5 R3.2 F117.
Y-1.
Y-.5
Y0.
Y.5
Y1.
Y1.5
X2.649 Y1.25
Y.75
Y.25
Y-.25
Y-.75
Y-1.25
X2.149 Y0.
Y-1.
Y-.5
Y.5
Y1.
Y1.5
Y-1.5
X1.649 Y1.25
Y.75
Y.25
Y-.25
Y-.75
Y-1.25
M11
X1.8069 Y-1.5 Z2.1113 B76.593 R2.8113
M10
Y-.5

And here is a video of the crash to go along with it: https://youtu.be/QWE6gMb8bqs

Drills the first 26 holes correctly no problems, as soon as it rotates the B axis, it breaks the drill, and plunges into the part. I contacted my Mastercam dealer and they fowarded all the information to Mastercam as they were unable to figure out the problem. They suggested that my Retract distance by higher. That would solve the tool breaking on the rotation of the B axis, but not that the drill plunged into the part. All the holes are set for -0.5".

All the vectors are pointing in the right direction. I was not using single block, I was on the 26th hole, but yes I should have been more careful.
I can provide the file for anyone that would like to take a look. Again, I could be completely missing a "check this box" as this is my first time trying this without creating a separate DWO for each angle.

 

[Dave_WDM]

I do 5 axis drilling a lot on a Fanuc control. It works great. Except that it cannot use TCP because TCP doesn't support canned cucles. Mine uses Tilted Working Plane and outputs a different G68.2 for each hole after returning Z Axis to home.

Do you know if this is true for HAAS as well? As my post definitely outputs a canned cycle.

 

[thesidetalker]

Okay here is the code:

G00 G17 G40 G80 G90 G93
(.283 TSC DRILL|TOOL - 13|DIA. OFF. - 13|LEN. - 13| DIA. - .28346457)
G53 Z0.
G53 Y0.
B0.
G53 X-23.
M11
M13
T13 M06
T10
G90 G54 C180. B90.
S9750 M03
M10
M12
G254 X3.149 Y-1.5
G43 H13 Z3.2
G94
G81 G99 Z2.5 R3.2 F117.
Y-1.
Y-.5
Y0.
Y.5
Y1.
Y1.5
X2.649 Y1.25
Y.75
Y.25
Y-.25
Y-.75
Y-1.25
X2.149 Y0.
Y-1.
Y-.5
Y.5
Y1.
Y1.5
Y-1.5
X1.649 Y1.25
Y.75
Y.25
Y-.25
Y-.75
Y-1.25
M11
X1.8069 Y-1.5 Z2.1113 B76.593 R2.8113
M10
Y-.5

And here is a video of the crash to go along with it: https://youtu.be/QWE6gMb8bqs

Drills the first 26 holes correctly no problems, as soon as it rotates the B axis, it breaks the drill, and plunges into the part. I contacted my Mastercam dealer and they fowarded all the information to Mastercam as they were unable to figure out the problem. They suggested that my Retract distance by higher. That would solve the tool breaking on the rotation of the B axis, but not that the drill plunged into the part. All the holes are set for -0.5".

All the vectors are pointing in the right direction. I was not using single block, I was on the 26th hole, but yes I should have been more careful.
I can provide the file for anyone that would like to take a look. Again, I could be completely missing a "check this box" as this is my first time trying this without creating a separate DWO for each angle.

Well the code is bad, no doubt about it. The post is not configured correctly. There should be a retract or a linking move on that hole at the new B-angle. You can't just call different B or C-angles willy nilly, while G254 is active.

You should only call different B-angles on drilling cycles if you're programming from center of rotation and not using G254. It appears you are programming to the part, so you should have G254 active.

It should retract some amount (either to G53 Z0, or using a TCPC G234 linking move to next position), then rotate to next hole position, then call a new G81

Your mastercam dealer can't see this?




For reference, DWO or G254 is for 3-axis milling at different angles, or 3+2. Position to new angle, call G254, then away you go. Before a new angle, cancel with G255 and then rotate, repeat.

G234 is for simultaneous milling, where the rotary axes can move at the same time with XYZ, but you can't use canned cycles, or G2/3 arcs, or 2d cutter comp G41/42, or some other things. Basically just G0 and G1.

Do you know if this is true for HAAS as well? As my post definitely outputs a canned cycle.

Yes it is similar. You can't use canned cycles in TCP (G234), it has to be in G254, which your post is outputting.

 

[thesidetalker]

Here's what your code should look similar to. This isn't from a MC program or post, but you should have similar output for your Haas. This code is from a cylindrical part with many holes around the outside.

With TCP link between holes:

T38 M6 (TOOL 38 - DRILL - CARB - 3.17MM 3XD TSC GUHRING 9055100031700) 
G0 G49 G90 G53 Z0
M11 
M13 
G0 G90 G54 B90. C-10.743 
M88 
G254 
M3 S5203 
G0 G90 X3.9375 Y0 
G43 H38 Z4.0995 
G0 Z4.0295 
G81 G98 X3.9375 Y0 Z3.8568 R4.0295 F20.812 
G80 
(DRILL .125 THRU) 
G255 
[B]G234 H38 X4.0277 Y-0.7642 Z-3.9375 
G1 G93 X3.9721 Y-1.0143 Z-3.9375 B90. C-14.325 F130.
G0 G90 G54 B90. C-14.325 
G49 [/B]
G254 
G0 G90 G94 G54 X3.9375 Y0 
G43 H38 Z4.0995 
G0 Z4.0295 
X3.9375 Y0 
G81 G98 X3.9375 Y0 Z3.8568 R4.0295 F20.812 
G80
..

And no TCP link, retracting to Z0:

T38 M6 (TOOL 38 - DRILL - CARB - 3.17MM 3XD TSC GUHRING 9055100031700) 
G0 G49 G90 G53 Z0
G0 G90 G54 B90. C-10.743 
M10 
M12 
M88 
G254 
M3 S5203 
G0 G90 X3.9375 Y0 
G43 H38 Z4.0995 
G81 G98 X3.9375 Y0 Z3.8568 R4.0295 F20.812 
G80 
(DRILL .125 THRU) 
G0 G49 G90 G53 Z0
G255 
G0 G90 G54 B90. C-14.325 
G254 
G0 G90 G54 X3.9375 Y0 
G43 H38 Z4.0995 
G81 G98 X3.9375 Y0 Z3.8568 R4.0295 F20.812 
G80
..