2018 BUG - 2D HIGH SPEED AREA MILL with TROPICAL MOTION

[PcRobotic]

Hello everyone,
      I just found out that MasterCam2018 has a bug of which I'm using 2D HIGH SPEED AREA MILL with TROPICAL MOTION turned on and if gave me a message of:

M00 (TOOL INSPECTION POINT - POST CUSTOMIZATION REQUIRED)

surely, I did not turn on the TOOL INSPECTION/ CHANGE mode on but the post gave me that message and weird M-CODES (Please see below).  I also tried the DEFAULT MasterCam post and these are the codes below.

       I maybe wrong of writing program (I hope), is there away I can fix it or it really a bug?

+++++++++++++++++++++++++++++++++

MCX FILE - Z:\CAD - CAM\JOBS\50-1327\50-1327-32C.MCAM)
(NC FILE - C:\USERS\ADMIN\DOCUMENTS\MY MCAM2018\MILL\NC\50-1327-32C OP2A.NC)
(MATERIAL - 6061-T6)
( T15 | 1/8 EM | H15 | XY STOCK TO LEAVE - .015 | Z STOCK TO LEAVE - .015 )
G20
G0 G17 G40 G49 G80 G90
( 2D HIGH PSEED TOOLPATH - AREA MILL )
T15 M6
G0 G90 G54 X-.4482 Y-1.5312 A0. S8500 M3
G43 H15 Z1. M8
Z.0625
G1 Z-.0341 F200.
G18 G3 X-.4634 Z-.0812 I-.0998 K.0062 =====> G18????
G1 X-.4707 Y-1.5313 Z-.0913
(CUTTING....)
G1 Y-.6005
Y-.5974 M00
M00 (TOOL INSPECTION POINT - POST CUSTOMIZATION REQUIRED)
X-.2839
G2 X-.2937 Y-.598 I-.0098 J.0809
X-.3742 Y-.5292 I0. J.0815
G1 X-.3749 Y-.4514
Y-.4477 M01
X-.7929 Y-.4474
G3 X-.7995 Y-.447 I-.0066 J-.0497
X-.8496 Y-.4971 I0. J-.0501
X-.8492 Y-.5028 I.0501 J0.
G1 Y-2.012
G3 X-.8494 Y-2.0169 I.0505 J-.0049
X-.7987 Y-2.0676 I.0507 J0.
X-.7929 Y-2.0674 I0. J.0507
G1 X-.3774
X-.375 M01
X-.3749 Y-1.9594
G2 X-.3753 Y-1.9514 I.0787 J.008
X-.3014 Y-1.8725 I.0791 J0.
G1 X-.1805 Y-1.8724
G3 X-.1758 Y-1.8677 I0. J.0047
X-.1805 Y-1.863 I-.0047 J0.
X-.1852 Y-1.8677 I0. J-.0047
X-.1805 Y-1.8724 I.0047 J0.
G1 X-.175
X-.1749 Y-1.0563
G0 Z1.
M5
G91 G28 Z0. M9
G28 X0. Y0. A0.
M30
%

 

==================================================

 

[huskermcdoogle]

Sample file?  Also this likely needs to be moved to industrial forum.   calling jparis....

[Tim Johnson]

I just ran into something similar yesterday in 2017. I've started training another programmer for horizontal work. I was showing him different options with boss/bore location finding and I turned on the extra drill parameters to show him how to set up three point probing, reset every thing back to 0 and turned parameter box off. When I posted the file the program had the three point probing installed. I ended up having to remove that operation and rewrite it to get it back to normal. Maybe the issue I had is a bug has been around for a while. Try renaming your file, delete and replace the operation and see if it fixes your problem. If it does then you have both files to send in to quality control.

[PcRobotic]

This toolpath is only happened on 2018 though. Area Mill 2D High Speed.

[Chris In-House Solutions]

Hey PcRobotic,

What post are you using?  Did you try this with the default post that comes with Mastercam2018?  Perhaps one of the parameters in the Area Mill toolpath got changed and your post needs to be modified?  I will test it once I get into the office this morning and let you know what I end up getting.  

[Chris In-House Solutions]

PcRobotic,

I used the generic post that came with Mastercam2018 and the latest mpmaster post and didn't get the same results as you.  I could be programming this toolpath slightly different than you which may result in different output.  Based on my test it seems your post may require a modification to not output that code.  

[Tim Johnson]

18 hours ago, PcRobotic said:

This toolpath is only happened on 2018 though. Area Mill 2D High Speed.

If you happened to click on the tool inspection box, played with it and then unclicked it that would be the same type of process that I did when I had the same type of issue you're having. I had to rewrite my operation to fix it.

[Chris In-House Solutions]

Hey Tim,

I got the same behavior as you are describing.  I will make a video up and send it into CNC Software.  PcRobotics can you confirm you did the same process as Tim describes above?

[jlw™]

Man, this is a bug every where.  I stay away from this like the plague.  It is especially wacky with my bought posts.  That's one thing I miss about Esprit, it handled this well.  I simply program around it making my ops run for the expected amount of time.  I often use canned text for hard M00 and I always output M01 so that the guy running it has the option to stop at every op.  The more flexibility you give to the man at the control panel, the better off both of you are.  I even program safe times so that if the tool doesn't need changing the can simply hit cycle start.

[gcode]

Odd.. I modified an HBM post to use Inspection Point back is X6 and have updated for every release

I just used it on an MC2018 project and it worked flawlessly

I have it set up on a couple of paid for 5X posts, and just used one of those with no trouble.

 

[Chris In-House Solutions]

Okay so now I cant re-create it to make a video or even a .MCAM file to send to CNC Software.  Even when I have tool inspection turned on the post actually will not output the "tool inspection point - post customization required".

[Tim Johnson]

Wow, That is weird.

When I had my issue Saturday I just attributed it to not shutting off/restarting my computer for a month. I didn't think about a bug.

Thanks for sending at least my issue in Chris.

[Chris In-House Solutions]

Tim Johnson,

I cant re-create the issue and if I cant re-create it I cant really send it in to CNC Software.  

[crazy^millman]

4 minutes ago, Chris Lang In-House Solutions said:

Tim Johnson,

I cant re-create the issue and if I cant re-create it I cant really send it in to CNC Software.  

It is nice you saw it. I hate seeing things QC cant reproduce. I send in videos and screen shots and still a lot of the time they never see it. I know what I see and yes I am crazy, but it is nice when someone else sees it. If two or more people smell smoke there is a good chance there is a fire.

[Chris In-House Solutions]

Maybe I need to re-start my computer to get it to re-produce but that doesn't really make sense to me.  I had the issue, deleted all the operations and started making a video without the tool inspection turned on and sure enough the tool inspection code came out in the posted code.  So I started a new session of Mastercam and when I did that I couldn't get the post to output the "tool inspection point - post customization required" output again.   

[crazy^millman]

10 minutes ago, Chris Lang In-House Solutions said:

Maybe I need to re-start my computer to get it to re-produce but that doesn't really make sense to me.  I had the issue, deleted all the operations and started making a video without the tool inspection turned on and sure enough the tool inspection code came out in the posted code.  So I started a new session of Mastercam and when I did that I couldn't get the post to output the "tool inspection point - post customization required" output again.   

Keep a file going for a while and you will start to see all kinds of things. Get the file above 200 mb and really fun things start popping up. Leave it running over a weekend on a large file and Monday will be full of surprises also.

[PcRobotic]

5 hours ago, Chris Lang In-House Solutions said:

Hey PcRobotic,

What post are you using?  Did you try this with the default post that comes with Mastercam2018?  Perhaps one of the parameters in the Area Mill toolpath got changed and your post needs to be modified?  I will test it once I get into the office this morning and let you know what I end up getting.  

 

I used the DEFAULT MACHINE DEFINITION and i checked, I only used in the one I have shown in the pictures.  

[Tim Johnson]

1 hour ago, Chris Lang In-House Solutions said:

Maybe I need to re-start my computer to get it to re-produce but that doesn't really make sense to me.  I had the issue, deleted all the operations and started making a video without the tool inspection turned on and sure enough the tool inspection code came out in the posted code.  So I started a new session of Mastercam and when I did that I couldn't get the post to output the "tool inspection point - post customization required" output again.  

That's what I did but inside the extra drill parameters (8,9 and 10).

[Chris In-House Solutions]

Tim Johnson what do you mean by extra drill parameters?   The Area Mill Toolpath doesn't have drill parameters.  Can you take a screen shot of what you mean?

Quote

That's what I did but inside the extra drill parameters (8,9 and 10).

 

[billb]

Thanks for bringing this issue to our attention.  It looks to me like the cutter comp and position code fields, in the binary nci, have uninitialized values in them, in MC2018 (and MC2019) when the Trochoidal Motion/Minimize Burial option is used.  I just used 2D HST Area mill and a rectangle with Trochoidal motion to see the issue.  I logged this as D-30834.

The binary nci records, with Trochoidal motion turned off, look good.

I think the problem is limited to 2D HST (the cutter comp and position code fields in 3D HST Area roughing look good).

[Tim Johnson]

2 hours ago, Chris Lang In-House Solutions said:

Tim Johnson what do you mean by extra drill parameters?   The Area Mill Toolpath doesn't have drill parameters.  Can you take a screen shot of what you mean?

 

Chris,

I was showing a programmer how to probe a part and my probing comes from the custom drills segment.