Forum Navigation
Please or Register to create posts and topics.

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

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

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.

 

Peter,

I'm willing to test Router post.

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

Regards,

Arie.

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.

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/topic/wanted-testers-for-new-fusion-360-post-processors-mill-plasma/?part=2#postid-12104

Uploaded files:

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

@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

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

@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.

@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.