MasterCAM 2022 Verification Unknown Error

[Myth Project]

Alright, I'm trying to program a part and I'm having issues while using the techniques I've used for years.  I'm attaching the file for reference.  I generally program my 4th axis through Transform Rotating Toolpaths and through creating different planes at the different angles.  I also will select drill toolpaths and enable Rotary Axis Control so that I can get all the holes around a part.  Sometimes I'll use the other, less practical methods, but not often.  In MCAM2022 I'm having issues running my verify.  It will verify all operations where the Rotary Axis Control is off (1-17), or the ones where it's on (18-20), but will error out when I try to verify all at once (1-20).  Any advice?

Example.mcam

[crazy^millman]

Start it one time and close the Mastercam. Try it again and see if that works. Other thing is to make sure your Graphics is not using the onboard Graphics card, but is using the Professional Video card for the system you have. Onboard card are problematic for Mastercam and High End cards should always be used for the best performance and reliability with Mastercam.

You have defined holes in different planes, but didn't set the operation up to be a Multiaxis drilling operation. It cannot verify what it cannot do. Yes it does backplot which is wrong it shouldn't allow you to backplot the operation since it probably doesn't even post correctly, but that is what happens when a Software is not Kinematic aware. See there are no rotations in the posted code. Either set it up correctly as a Multiaxis operation in the drill cycle or do what you were doing with the milling and using X form to rotate the toolpaths.

O0000(EXAMPLE)
(DATE=DD-MM-YY - 03-12-21 TIME=HH:MM - 08:44)
(MCAM FILE - C:\USERS\RON\APPDATA\LOCAL\TEMP\EXAMPLE.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\EXAMPLE.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T4 | 1/8 C'DRILL | H4 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
( SPOT DRILL HOLES )
N120 T4 M6
N130 G0 G90 G59 X-.975 Y-.1152 A0. S2100 M3
N140 G43 H4 Z2.5145 M8
N150 Y1.
N160 Z2.31
N170 G98 G82 Z.43 R.6 P.05 F2.
N180 G80
N190 X-1.25 Y.3476
N200 Z.8379
N210 G98 G82 Z-1.0421 R-.8721 P.05 F2.
N220 G80
N230 Z.91
N240 Y-.9
N250 G98 G82 Z-.97 R-.8 P.05 F2.
N260 G80
N270 Z1.31
N280 X-.975 Y-1.
N290 G98 G82 Z-.57 R-.4 P.05 F2.
N300 G80
N310 Z2.7873
N320 X-1.25 Y-.4773
N330 G98 G82 Z.9073 R1.0773 P.05 F2.
N340 G80
N350 M5
N360 G91 G28 Z0. M9
N370 G28 X0. Y0. A0.
N380 M30

 

[crazy^millman]

With the operation setup to use the features from the solid, 4 Axis along X and use TOP of Holes for depth settings it Verifies and posts the correct code. I changed the OP19 and OP20 to be 4 Axis toolpaths and got them to Verify. You did have them setup correctly and not sure why it wouldn't verify them, but changing them allowed everything to Verify.

%
O0000(EXAMPLE)
(DATE=DD-MM-YY - 03-12-21 TIME=HH:MM - 08:57)
(MCAM FILE - C:\USERS\RON\APPDATA\LOCAL\TEMP\EXAMPLE.MCAM)
(NC FILE - C:\USERS\RON\DOCUMENTS\MY MASTERCAM 2022\MASTERCAM\MILL\NC\EXAMPLE.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T4 | 1/8 C'DRILL | H4 )
N100 G20
N110 G0 G17 G40 G49 G80 G90
( SPOT DRILL HOLES )
N120 T4 M6
N130 G0 G90 G59 X-1.25 Y.3536 A-315. S2100 M3
N140 G43 H4 Z2.84 M8
N150 G98 G82 Z.96 R1.13 P.05 F2.
N160 X-.975 Y-.5 Z.93 A-90. R1.1
N170 X-1.25 Y.185 Z.9463 A150. R1.1163
N180 Y0. Z1.2028 A225. R1.3728
N190 X-.975 Y-.5 Z.93 A270. R1.1
N200 G80
N210 M5
N220 G91 G28 Z0. M9
N230 G28 X0. Y0. A0.
N240 M30
%

Do me a favor and take the time to define your holders. Trust me once you get in the habit of doing so and getting exact results for your machining you will never not want to spend the extra time doing so.

 

 

[crazy^millman]

Sorry, but I am about to come across as a pain and know it all.

Why is the endmill feeding at .0011 per inch and it is a rougher? Why are you stepping down verse using Dynamic to machine this part? The run time on the part using those speeds and feeds is 35mins probably more like 40+ minutes. With Dynamic and some other thing you can get this run time down to under 15 minutes. If you will provide me the material you are cutting and the EDP numbers of the tools you are using along with the machine information I will be glad to show you exactly what I am talking about to improve your run time. We are not going to compete with China cutting parts like that.

You have 300 sfm on the endmill that is carbide you should be able to run the same SFM on the drills. With through the spindle coolant there is no need to peck those drills. There are other things to improve this also. Facing the small chamfers you can single contour them and make that one pass. Backplot says 27 seconds, but on the machine thinking more like 1 minute with all those rapid and retract moves for face each one. Once pass less than 10 seconds on each smaller face. One the larger one can dynamic it at about the same time, but since you were plowing through the material anyway then one passing those would work. Another 3 minutes reduction in run time.

[Myth Project]

Odd, when I post only the center drill, (operation 18), this is what I get... 

%
O0000(MC2022)
( T4 | 1/8 C'DRILL | H4 )
G20
G0 G17 G40 G49 G80 G90
( SPOT DRILL HOLES )
T4 M6
G0 G90 G59 X-.975 Y-.5 A90. S2100 M3
G43 H4 Z1.81 M8
G98 G82 Z.93 R1.1 P.05 F2.
X-1.25 Y.185 Z.9456 A150. R1.1156
Y0. Z1.2028 A225. R1.3728
X-.975 Y-.5 Z.93 A270. R1.1
X-1.25 Y.3536 Z.9586 A315. R1.1286
G80
M5
G91 G28 Z0. M9
G28 X0. Y0. A0.
M30
%
 

So, I'm not sure what's different in what we are looking at.

[Myth Project]

1 minute ago, crazy^millman said:

Sorry, but I am about to come across as a pain and know it all.

Why is the endmill feeding at .0011 per inch and it is a rougher? Why are you stepping down verse using Dynamic to machine this part? The run time on the part using those speeds and feeds is 35mins probably more like 40+ minutes. With Dynamic and some other thing you can get this run time down to under 15 minutes. If you will provide me the material you are cutting and the EDP numbers of the tools you are using along with the machine information I will be glad to show you exactly what I am talking about to improve your run time. We are not going to compete with China cutting parts like that.

You have 300 sfm on the endmill that is carbide you should be able to run the same SFM on the drills. With through the spindle coolant there is no need to peck those drills. There are other things to improve this also. Facing the small chamfers you can single contour them and make that one pass. Backplot says 27 seconds, but on the machine thinking more like 1 minute with all those rapid and retract moves for face each one. Once pass less than 10 seconds on each smaller face. One the larger one can dynamic it at about the same time, but since you were plowing through the material anyway then one passing those would work. Another 3 minutes reduction in run time.

Yeah, contouring the chamfers may be a better, just need to make sure there is enough clearance with my 4th axis and fixturing to achieve it without issue.  The material is 45HRC 13-8, work holding rigidity is he issue with pushing hard.  Can it be pushed harder? Yes.  I need one good part for the order.  If I push it and it fails, I saved no time.  I do understand what you are saying, but I do not work for a production shop, we are prototype with crazy materials and tough tolerances.  I truly believe most shops no quote the jobs we get...

All that said, I do very much appreciate any and all advice about machining practices, so you haven't offended me at all.  I'm not the sensitive type of machinist.  I will also look at Dynamic milling the faces, see what it'll look like.  Thanks for the insight!

[crazy^millman]

15 minutes ago, Myth Project said:

Odd, when I post only the center drill, (operation 18), this is what I get... 

%
O0000(MC2022)
( T4 | 1/8 C'DRILL | H4 )
G20
G0 G17 G40 G49 G80 G90
( SPOT DRILL HOLES )
T4 M6
G0 G90 G59 X-.975 Y-.5 A90. S2100 M3
G43 H4 Z1.81 M8
G98 G82 Z.93 R1.1 P.05 F2.
X-1.25 Y.185 Z.9456 A150. R1.1156
Y0. Z1.2028 A225. R1.3728
X-.975 Y-.5 Z.93 A270. R1.1
X-1.25 Y.3536 Z.9586 A315. R1.1286
G80
M5
G91 G28 Z0. M9
G28 X0. Y0. A0.
M30
%
 

So, I'm not sure what's different in what we are looking at.

No sure either. I took what was put up and posted it. Maybe you caught the mistake and had already fixed it.