Wanted testers for new Fusion 360 Post processors. Mill & Plasma

[masso-support]

Hi Guy's

Have been working with Will from Autodesk developing some new post processors and am now looking for some testers to try them out. I'm afraid I don't know anything about Fusion myself.

If you would like to try out the new posts please leave your comment here and which version you would like to try and I will get you the post to try out. All you need to do is try it out and let me know how it goes. If you find issues I will forward them to Autodesk.

It will be much appreciated.

Cheers Peter



PS if you are a lathe user there was a new Lathe Post processor release a couple of months ago.

https://cam.autodesk.com/hsmposts?p=masso_turning

 

[shine-on]

I use Fusion 360 exclusively for all my cnc machines. 3D printer, Glowforge laser cutter, and my router. I am quite familiar with G code and use a text editor with macros to edit the current stock Fusion 360 post processor.

I would be happy to try out anything new, but I must admit that the current post on Fusion does most everything I need for my router with a manual tool change.

 

[breezy]

Peter,

I'm willing to test Router post.

I will compare it to the MASSO version that I created.

Regards,

Arie.

 

[peter35]

Peter, would be happy to run on my milling machines. 5A-2798 4 axis.

Have been using fusion with masso for the last couple of years.

 

[cncnutz]

Thanks Guys, I really appreciate it.

@shine-on @breezy @peter35

Looks like you are all router users so I have attached the post for Mill below. I believe it is capable of creating sub routines in the correct format needed.

Just be careful when using in case there are issues.

Let me know your feedback and any problems you might find.

Cheers Peter



Are there any Plasma users who want to Try the new plasma Post? Get em while their hot!

Plasma post processor now on post #15 https://www.masso.com.au/forums/top...t-processors-mill-plasma/?part=2#postid-12104

 

[peter35]

Mill 4 axis V3.44

Have just machined 20 small parts, one setup with 4 operations, all drill cycles and different tooling.

Using F4 toolset without ATC.

Removed G53 code from program.

No problems, have another job to run tomorrow which is similar.

Peter

 

[testyourdesign]

@cncnutz

I already modified my Fusion post to remove some of the G-Codes that are not used by Masso. I wouldn't mind testing it on my Mill but can you describe what changes they di to the posts?

Cheers, Stephen Brown

 

[cncnutz]

Thanks for the update @peter35

Hi Stephen,

You are more than welcome to try out the new Post Processor. Just grab the file from post #5

I would be lying if I said I knew for sure. I sent information on how it worked and reviewed some Gcode test samples that were created and sent back. Not as good as using it myself and creating files for machining but it would take me too long to learn to use it so I turn to you to tryout.

Mill Post Processor: All unsupported codes have been removed from the post processor. When making a program with subroutines it should create the subroutine programs as separate files instead of adding them to the end of the gcode file. It should support 5 axis and 3+2 axis 5 axis machining.

Plasma Post Processor: Unsupported codes removed, Probing G38.2 added, Masso M666 & M667 THC commands added.

Cheers Peter

 

[breezy]

@cncnutz

Peter,

I'm unable to test changes on the BMS machine as I've self isolated because of the COVID-19 situation ( which is not bad here in Perth), but have checked against Gcode produced by my version of PP and the only difference is in spacing of blank lines that I added to my version and the position of the G28 safe retract code appears in the output code, which is better placed.

As the official version from Autodesk does not include pass through function code which I had added to my version, I added it to the version I received from you and compared the results to code that I have used in the past and found it to be the same, bar what I've already mentioned. Fusion allows additional manual code insertion by using a menu item Manual NC, this has 20 fixed Gcode codelets and one that is called Pass Through that allow you to write your own Gcode that can be inserted into the resultant output code. For this to work the following needs to be added in three places in the pp.

passThroughManualCommands: true // Allows manual command to be entered in Fusion.​

passThroughManualCommands: {title: "Manual Commands", description: "Set to true to allow Manual Fusion Commands to inputted into Gcode.", type: "boolean"}​

/**
Enter manual processor commands.
*/
function onPassThrough(text) {
if (properties.passThroughManualCommands) {
var commands = String(text).split(",");
for (text in commands) {
writeBlock(commands[text]);
}
}
}​

The first is added to the users properties structure, second to the propertyDefinitions structure and the last part is the function that performs the action.

Other things that I noticed is the option to include tool change has been removed and is now a default function, 5 axis machining code, removal of rigid tapping, addition of looping on M30 and minor order adjustments ie comments after Gcode action.

As I don't use any 4 or 5 axis machining I can't comment on that.

Regards,

Arie.

 

[breezy]

@cncnutz

Peter,

Had a further play with Fusion and the new PP, in particular subroutines, which I haven't used before, and I'm impressed with the results. When tried this with my version of PP it resulted in all the subroutines being included at the bottom of the calling file.

A feature that could be added is the ability to set the starting number of the subroutine file name. This will allow testing of changes to the manufacture toolpaths without over writing previous versions or the need to store in a different folder. I added and tested this feature and it works great. It will require the addition to the properties, propertyDefinitions structures and the setting of the lastSubprogram value.

subroutineNumberStart: 1000 // first subroutine number​

subroutineNumberStart: {title:"Start subroutine number", description:"The number at which to start the subroutine numbers.", group:1, type:"integer"}​

lastSubprogram = properties.subroutineNumberStart;​

It will be a while before I can visit the BMS machine to test the performance of the subroutine version to the original version, that I have used.

Hopefully you can get Autodesk to include this and my previous post's feature to all versions of the MASSO PP.

Regards,

Arie.

 

[pablo-olivas]

Hi

I try the post processor for plasma, but this error appear:

Error: Waterjet, laser, and plasma cutting toolpath are not supported by the post configuration.
Failed while processing onOpen().

What could be happening?

 

[masso-support]

Hi Pablo,

The post Processor I uploaded was for Mill only. The Plasma Post has been attached below.

Let me know how it goes.

Cheers Peter

Plasma post processor for testing is now on Post #15 https://www.masso.com.au/forums/top...t-processors-mill-plasma/?part=2#postid-12104

 

[masso-support]

@testyourdesign @shine-on @peter35 @breezy

Hi guys

Hope all is good with you. Just wondering it you have had a chance to test the new Mill Post Processor and if you had any comments or suggestions you would like to pass on to Autodesk.

Arie has already given some suggestions that I have passed on but if you have found anything wrong or missing, speak now of forever hold your peace. ;-)

Cheers Peter

 

[breezy]

Peter,

Haven't spent any more time on the PP but will test any updates that you bring forward.

I'm not an expert on Fusion but I'm satisfied with the changes that I inserted into the PP. I haven't had a chance to test the resultant Gcode on the BMS MASSO, but the previous version didn't have any gotas in it. Any failures that I had were caused by operator error, either on the machine or in programing the toolpath in Fusion.

Fusion has grown to be beyond what a hobbyist would need as it has moved into the realm of big business and as a result it has a lot of features that are not needed for milling work.

Regards,

Arie.

 

[masso-support]

@breezy

Thanks Arie, Your input is always much appreciated .

@pablo-olivas

Autodesk have sent me the revised post processor for Plasma.
There is now a Safe Retracts property to choose to output G28 or G53 at the end of the program if desired and they also added the workOffset.

Anyone who wants to try it is welcome, Just let me know how it goes and any suggestions or problems you find.

Cheers Peter

 

[ecs]

Quote from MASSO Support on March 16, 2020, 7:27 pm

Hi Guy's

Have been working with Will from Autodesk developing some new post processors and am now looking for some testers to try them out. I'm afraid I don't know anything about Fusion myself.

If you would like to try out the new posts please leave your comment here and which version you would like to try and I will get you the post to try out. All you need to do is try it out and let me know how it goes. If you find issues I will forward them to Autodesk.

It will be much appreciated.

Cheers Peter



PS if you are a lathe user there was a new Lathe Post processor release a couple of months ago.

https://cam.autodesk.com/hsmposts?p=masso_turning

Hi Peter,

I got around to trying the lathe post processor and am having trouble. Its uses the G97 to turn on and off the constant surface speed. When the machine heads for a tool change and gets given G97 S1600 just before the tool change the machine spins up instead of stopping.

Shouldn't it be G96 to turn on and G97 to turn off? I tried changing it manually but still takes off when given G97 S1600

It also has a M3 when it probably should have a M5?

Maybe i'm doing something wrong?

My file generated from fusion using the masso post.

Regards,
Josh

 

[masso-support]

Hi @ecs

Thanks for the file Josh. I can see what you are talking about and I can see that all G96 & G97 are immediately followed by an M3.

The addition of the M3 after the G97 makes no difference because as soon as the G97 S1600 is issued to turn off CCS the spindle changes to the specified speed of 1600 so it ramps up regardless.

In the case of tool change the T2 M6 stops the spindle so an M5 is not needed.

It is possible that I am missing something as I don't use lathe myself. Let me know if I'm wrong.

Cheers Peter

 

[ecs]

@masso-support

Hi Peter,

I'm no expert so you'd know more than me but that sounds right and also explains why these things have been happening.
Can you let me know when its fixed so i can download it again and try it out?

Thanks for your help!

Thanks,
Josh

 

[masso-support]

Hi Josh

I'm not sure if change needs to be made to the Post processor.

The G97 turns off constant surface speed and the spindle changes back to 1600rpm which is why it ramps up especially if you were on the outside turning diameter.

Are you turning off the G96 when you do the tool change or is it automatic? Is there a setting in Fusion to leave Constant surface speed on or to set a new lower spindle speed when it exits CSS?

I don't use Fusion so don't know what the settings are. Hopefully someone who uses it can jump in and enlighten us.

Cheers Peter

 

[ecs]

Hi Peter,

I'm not aware of any settings but again i'm a newbie in this area.

I will take a video of the process to show how it works. Maybe its operating correctly and I just have a different view of how things should work. I just dont see why it would need to speed up as it goes for a tool change. I think a video will be best so you can see what i'm seeing.

Cheers,
Josh