Masso plasma post
- Thread starter justingro
- Start date
breezy
Moderator
@justingro
Justin,
Can you place a link to the post processor here so I can have look at it. Also attach the log file.
Regards,
Arie.
Justin,
Can you place a link to the post processor here so I can have look at it. Also attach the log file.
Regards,
Arie.
breezy
Moderator
Justin,
When Fusion failed to produce the Gcode it opened you editor with the log file, but it also stored it in the directory that you had directed it to put the resultant NC file. It will have a file extension of FAILED.
By the way Peter will be in bed at this time of night, unless he is an night owl!!!
Regards,
Arie.
When Fusion failed to produce the Gcode it opened you editor with the log file, but it also stored it in the directory that you had directed it to put the resultant NC file. It will have a file extension of FAILED.
By the way Peter will be in bed at this time of night, unless he is an night owl!!!
Regards,
Arie.
breezy
Moderator
Justin,
From what I can make out off the photo and looking at the PP code, you have Radius Compensation turned on in Fusion.
At the point of failure Fusion is checking what to do with radius compensation when it is travelling in a straight line, because it says there is radius compensation it goes into a portion of code where the next line says to throw an error, which causes it stop processing. Last thing it does before quitting is insert the M30 command to close the file that it has generated to that point.
Hope this helps you where to look in Fusion to fix the fault.
Regards,
Arie.
PS I'm off to bed now.
From what I can make out off the photo and looking at the PP code, you have Radius Compensation turned on in Fusion.
At the point of failure Fusion is checking what to do with radius compensation when it is travelling in a straight line, because it says there is radius compensation it goes into a portion of code where the next line says to throw an error, which causes it stop processing. Last thing it does before quitting is insert the M30 command to close the file that it has generated to that point.
Hope this helps you where to look in Fusion to fix the fault.
Regards,
Arie.
PS I'm off to bed now.
hi Peter had a go at your post you sent me on a basic square and two things came out
- there is no G28 code to return to home position at end of cut
- there is also no G 38.1 for torch zero for floating head
- I had problems with the G54 code even when i zeroed my dro the machine would still go to my g54 saved location every time when pressing cycle start with the masso fusion 360 program i could zero my dro and start cut from that position added both g code files Justin
Attachments
breezy
Moderator
@justingro
Justin,
Check the properties box when you call up the post processor, in there look for useZAxis this is set to false by default, try with it set to true.
Instead of taking photos of your code, it is hard to read, post the actual file to the message, file upload will accept the following
jpg,jpeg,gif,png,bmp,pdf,cnc,tap,htg,nc,scpost,zip
These have been taken from the list below when in reply mode.
Have you fixed your homing setup, until you sort that out, you will have problems with G54.
In the Fusion file you are using G53 Move In Absolute Machine Coordinates which will override any DRO zeroing you are doing and NO G54.
Regards,
Arie.
Justin,
Check the properties box when you call up the post processor, in there look for useZAxis this is set to false by default, try with it set to true.
Instead of taking photos of your code, it is hard to read, post the actual file to the message, file upload will accept the following
jpg,jpeg,gif,png,bmp,pdf,cnc,tap,htg,nc,scpost,zip
These have been taken from the list below when in reply mode.
Have you fixed your homing setup, until you sort that out, you will have problems with G54.
In the Fusion file you are using G53 Move In Absolute Machine Coordinates which will override any DRO zeroing you are doing and NO G54.
Regards,
Arie.
Hi @justingro
I've been playing with fusion and finally managed to get some gcode out of it. I have posted my first feeble attempt below.
Arie is correct that you have radius compensation turned on. I had the same problem and had to set compensation to in computer.
You also have to turn to probing to get the G38.2 probing cycle and set parameters.
@breezy
How's everything over there with you. Did I see somewhere you were in isolation at the moment? Hope you and your family are all ok.
Cheers Peter
I've been playing with fusion and finally managed to get some gcode out of it. I have posted my first feeble attempt below.
Arie is correct that you have radius compensation turned on. I had the same problem and had to set compensation to in computer.
You also have to turn to probing to get the G38.2 probing cycle and set parameters.
@breezy
How's everything over there with you. Did I see somewhere you were in isolation at the moment? Hope you and your family are all ok.
Cheers Peter
Attachments
breezy
Moderator
@cncnutz
Peter,
The other thing that needs to be turn on is use Z axis. To me it seems Autodesk set the plasma post to conservative mode as default. So users of the post need to go through all of the properties to set it to the way they it to produce their Gcode. Or if they are adventurous edit the post processor code to set the properties directly.
Here is the portion of code that will need tweaking.
Regards,
Arie.
We're well, I've placed myself & wife into "self isolation" by restricting travel to essential only. The family is good, they are returning to Karratha on Sunday, been in Perth for the last two weeks for the birth of 4th grandchild, but haven't seen them since they arrived, because of government advice for those over 60 stay away from children who could be carrying the virus without symptoms.
The number of cases here in WA have ramped up in the last two days, 30 compared to 35 in the last three weeks.
Peter,
The other thing that needs to be turn on is use Z axis. To me it seems Autodesk set the plasma post to conservative mode as default. So users of the post need to go through all of the properties to set it to the way they it to produce their Gcode. Or if they are adventurous edit the post processor code to set the properties directly.
Here is the portion of code that will need tweaking.
// user-defined properties
properties = {
writeMachine: true, // write machine
showSequenceNumbers: true, // show sequence numbers
sequenceNumberStart: 10, // first sequence number
sequenceNumberIncrement: 5, // increment for sequence numbers
separateWordsWithSpace: true, // specifies that the words should be separated with a white space
pierceDelay: 1, // specifies the delay to pierce in seconds
probeOffset: 0, // specifies the offset for G38.2 probing
probe: false, // probing
useZAxis: false, // specifies to enable the output for Z coordinates
pierceHeight: 0, // specifies the pierce height
useG0: true, // toggle between using G0 or G1 with a highFeedrate for rapid movements
looping: false, // output program for M98 looping
numberOfRepeats: 1, // specifies times to loop program
useParenthesesForComments: true, // specifies output of '()' or '#'
minTHCFeed: (unit == MM ? 500. : 20.) // minimum feed to output M666 THC
};
properties = {
writeMachine: true, // write machine
showSequenceNumbers: true, // show sequence numbers
sequenceNumberStart: 10, // first sequence number
sequenceNumberIncrement: 5, // increment for sequence numbers
separateWordsWithSpace: true, // specifies that the words should be separated with a white space
pierceDelay: 1, // specifies the delay to pierce in seconds
probeOffset: 0, // specifies the offset for G38.2 probing
probe: false, // probing
useZAxis: false, // specifies to enable the output for Z coordinates
pierceHeight: 0, // specifies the pierce height
useG0: true, // toggle between using G0 or G1 with a highFeedrate for rapid movements
looping: false, // output program for M98 looping
numberOfRepeats: 1, // specifies times to loop program
useParenthesesForComments: true, // specifies output of '()' or '#'
minTHCFeed: (unit == MM ? 500. : 20.) // minimum feed to output M666 THC
};
Regards,
Arie.
We're well, I've placed myself & wife into "self isolation" by restricting travel to essential only. The family is good, they are returning to Karratha on Sunday, been in Perth for the last two weeks for the birth of 4th grandchild, but haven't seen them since they arrived, because of government advice for those over 60 stay away from children who could be carrying the virus without symptoms.
The number of cases here in WA have ramped up in the last two days, 30 compared to 35 in the last three weeks.
@breezy
Sorry to hear that Arie. All that way and not getting to see them. Congratulations on the new addition though.
We have just hit 39 confirmes cases in NZ, 11 new today. Hope it can be kept under control as these things get out of hand really quick.
This weekend I plan to sit out on front porch in my rocking chair, Shot gun in hand, Banjo music playing in the back ground and protect my roll of Toilet paper.
Look after yourself
Cheers Peter
Sorry to hear that Arie. All that way and not getting to see them. Congratulations on the new addition though.
We have just hit 39 confirmes cases in NZ, 11 new today. Hope it can be kept under control as these things get out of hand really quick.
This weekend I plan to sit out on front porch in my rocking chair, Shot gun in hand, Banjo music playing in the back ground and protect my roll of Toilet paper.
Look after yourself
Cheers Peter
@justingro
More than i can tell you Justin. My total time with Fusion is a few hours today. By comparison you are a seasoned veteran.
I have been looking at the post processor and it looks like it can only outputs G53 which is what is screwing you up. I compared it to the Mill Post and there is some work offset calculations going no but not in the Plasma one. I will chase this up with AutoDesk and see if they can look at it. In the meantime you can edit the G53 and change it to G54 which will solve the issue you are having with your table. I just don't know about G28. There is plenty of mentions of it in the Mill Post processor but I don't see any in the Plasma. Maybe someone will point out a setting that needs to be set but in the meantime I have made a note of this as well to send to Autodesk.
Cheers Peter
More than i can tell you Justin. My total time with Fusion is a few hours today. By comparison you are a seasoned veteran.
I have been looking at the post processor and it looks like it can only outputs G53 which is what is screwing you up. I compared it to the Mill Post and there is some work offset calculations going no but not in the Plasma one. I will chase this up with AutoDesk and see if they can look at it. In the meantime you can edit the G53 and change it to G54 which will solve the issue you are having with your table. I just don't know about G28. There is plenty of mentions of it in the Mill Post processor but I don't see any in the Plasma. Maybe someone will point out a setting that needs to be set but in the meantime I have made a note of this as well to send to Autodesk.
Cheers Peter
testyourdesign
testyourdesign
@cncnutz
Have you tried the Microsoft Visual Studio Code (VSC) software yet? AutoDesk developed a plug-in for VSC that allows you to quickly and easily adjust the HSM/Fusion360 Post Processors. They included a debugger with sample code for cutting post processors with it as well. So far it only lists waterjet but it might be a useful tool for what you are doing. NYC-CNC posted a video on how to set it up. Best of all its free!
Cheers, Stephen Brown
Have you tried the Microsoft Visual Studio Code (VSC) software yet? AutoDesk developed a plug-in for VSC that allows you to quickly and easily adjust the HSM/Fusion360 Post Processors. They included a debugger with sample code for cutting post processors with it as well. So far it only lists waterjet but it might be a useful tool for what you are doing. NYC-CNC posted a video on how to set it up. Best of all its free!
Cheers, Stephen Brown
Attachments
breezy
Moderator
Stephen,
I've played with it, but haven't been able get the debugging part of it working. It will throw sample code out for certain operations, but you can't, at least I can't get it link produced Gcode back to the section of the post processor that produced it.
I'm currently sticking to Notepad++ which I'm very familiar with.
Regards,
Arie.
breezy
Moderator
@justingro
Justin,
Had a play with the masso plasma post to added G28 to it. Got it working but it may not be the correct way to do it, but I've attached it if you want to try it. Along with my output.
I've also turned on probe, use z and changed G53 to G54, but was not the correct way to do it, I didn't want to spend more time on it. You will need to set probe offset, pierce height & pierce delay in the properties.
Have fun testing.
Regards,
Arie.
Justin,
Had a play with the masso plasma post to added G28 to it. Got it working but it may not be the correct way to do it, but I've attached it if you want to try it. Along with my output.
I've also turned on probe, use z and changed G53 to G54, but was not the correct way to do it, I didn't want to spend more time on it. You will need to set probe offset, pierce height & pierce delay in the properties.
Have fun testing.
Regards,
Arie.