SolidCam Post processor

[MaccaRnD]

Just wondering if anyone has a post processor that works for Masso from solidworks/Solidcam

 

[ross-n]

Hi Macarms

I suggest you read through this post. It's not quite what you are hoping for, but I have found it useful:

Search results for query: solidworks-post-processor/

www.masso.com.au

 

[john-w]

Was just experimenting with the PP's which come with SolidworksCam 2020. The Haas VF3 PP seems to work fine with simple 2,5 D jobs.
In Machine Definitions / Posting / set output subroutines to NO and uncheck box "output subroutines for patterned features"
Possibly there is a solution for You, please let me know.

regards John

 

[MaccaRnD]

I’m still a few weeks away from
Cutting anything, haven’t tried loading any G code yet, still trying to get the machine to function as it should. Keen to make some chips

 

[JackRussel]

Hi Macarms

I suggest you read through this post. It's not quite what you are hoping for, but I have found it useful:

https://www.masso.com.au/forums/topic/solidworks-post-processor/#postid-17332-bp

It directs me to search the site, not a specific post...

 

[breezy]

It directs me to search the site, not a specific post...

That's because it is a link to the old forum
masso.com.au/forums/topic/solidworks-post-processor
Notice the structure of the link is different to the current link.
forums.masso.com.au/threads/solidworks-post-processor

solidworks post processor

hello,i am using solidworks for most 3d parts i am modelling.what post processor should i use for masso cnc mill? there is no masso in solidworks lists. is there any general purpose post procesor that works with masso or it doesnt matter what procesor i am using in solidworks? thanks!

forums.masso.com.au

 

[MaccaRnD]

Trying to Get this Sorted, I'm going to look at making a post processor to suit Solidcam. I have some Gcode I would like to machine, so I'm revisiting the Solidcam route and trying to generate something that Masso can work with. Initially I'm just after a few lines of code to machine a few radius on a part. But once that job is sorted I will be looking more in depth into an umbrella tool changer post processor and then move from the 3 axis to the 3 +2 and the hopefully the full 5 axis simultaneous PP. I think Solidcam has the ability to handle the knematics required (I don't know what I'm talking about).

 

[MaccaRnD]

here is some generated code for a basic 3 axis machine through Solidcam

N1 G90 G17 G40 G80 G00
N108 M06 T1 ()
N110 (F-contour3)
N112 G00 G54 G90 X16.9296 Y-7.6937 S3500 M03
N114 G43 H1 Z100.
N116 S3500
N118 Z100.
N120 Z2.
N122 G01 Z-8.2 F300.
N124 X17.3842 Y-7.302 F1000.
N126 G03 X16.9741 Y-7.0953 I-0.4545 J-0.3917
N128 G02 X10.4 Y-0.0021 I0.5259 J7.0805
N130 X16.7292 Y7.0865 I7.0999 J0.0306
N132 G03 X17.1319 Y7.3072 I-0.0651 J0.5965
N134 G01 X16.6641 Y7.6829
N136 G00 Z50.
N138 X16.9296 Y-7.6937
N140 Z2.
N142 G01 Z-8.2 F300.
N144 X17.5357 Y-7.1715 F800.
N146 G03 X16.9889 Y-6.8959 I-0.606 J-0.5222
N148 G02 X10.6 Y-0.0019 I0.5111 J6.881
N150 X16.751 Y6.8877 I6.8999 J0.0303
N152 G03 X17.2879 Y7.182 I-0.0868 J0.7953
N154 G01 X16.6641 Y7.6829
N156 G00 Z50.

 

[breezy]

Quick look spotted three problems with your code.

N108 M06 T1 () <===== Tool change order incorrect -- Should be Txx M06
N110 (F-contour3)
N112 G00 G54 G90 X16.9296 Y-7.6937 S3500 M03
N114 G43 H1 Z100. <===== Unsupported code MASSO will ignore entire line.
N116 S3500
N117 M03 <===== Missing M03 to start spindle
N118 Z100.

Just needs a M05 & M30 to finish off. Spindle OFF & Program end

 

[MaccaRnD]

That was just a snippet of the code there is that at the end

 

[MaccaRnD]

If that’s the case then for basic stuff just standard 3 axis post will work, I haven’t had a look at the tool changer side of things yet

 

[breezy]

That was just a snippet of the code there is that at the end

Although the tool change just before the end of program is strange. If the current tool is the tool requested G3 will ignore the command.

I haven’t had a look at the tool changer side of things yet

Issuing tool number after tool change command will preload the tool change function with the tool number for the next tool change command and you may not get the expected tool loaded.
eg.
MASSO remembers last tool number loaded between power cycles.
Current tool T1 following code will not load T2 until third M06.
M06 T1 <== No tool number to load, skips command and preload T1
...
M06 T2 <== T1 already loaded, skips command and preload T2
...
M06 T3 <== Loads T2 and preload T3

Current tool T1 following code will load T2 as expected.
T1 M06 <== T1 already loaded, skips command
...
T2 M06 <== Loads T2
...
T3 M06 <== Loads T3

 

[MaccaRnD]

Although the tool change just before the end of program is strange. If the current tool is the tool requested G3 will ignore the command.

Issuing tool number after tool change command will preload the tool change function with the tool number for the next tool change command and you may not get the expected tool loaded.
eg.
MASSO remembers last tool number loaded between power cycles.
Current tool T1 following code will not load T2 until third M06.
M06 T1 <== No tool number to load, skips command and preload T1
...
M06 T2 <== T1 already loaded, skips command and preload T2
...
M06 T3 <== Loads T2 and preload T3

Current tool T1 following code will load T2 as expected.
T1 M06 <== T1 already loaded, skips command
...
T2 M06 <== Loads T2
...
T3 M06 <== Loads T3

 

[MaccaRnD]

Attached is some of the options for the Post processsor I’m working through, if you see something that looks wrong can you please notify me, there’s a lot here I don’t understand, and obviously there is some functions Masso will not support

 

[MaccaRnD]

I won’t have time to run any tests on the mill till towards the end of next week, unforturntly the days don’t have 36hrs in them, it’s been a while but slowly getting my head back around the cam side of things. If I can get a funtional
PP working and start making some swarf I’ll then start to look at getting the orientation programming sorted with my spindle so I can do tool changes (at the moment I have to manually line up the tool so they can get loaded into the umbrella as there is no 0 or 180 degree alignment of the drive lugs on the BT40 tool holders,

 

[breezy]

Attached is some of the options for the Post processsor I’m working through

Seeing those screenshots reminded me of an attempt I tried several years ago to create a SolidCam PP to post on the forum, I couldn't make sense of the PP compiler, there wasn't any documentation on what did what.
I don't know if I still have all the software to compile a PP.

if you see something that looks wrong can you please notify me, there’s a lot here I don’t understand, and obviously there is some functions Masso will not support

You need to check G & M commands against the list in the MASSO documentation. Add what is missing and remove anything that is not supported.
In 5868 image you need to remove Tool Preload from the Section list.
In 5860 image you need to set Macro calls to False.

 

[MaccaRnD]

I haven’t yet worked out how to get the PP I’m working on to be the one it references off when it generates Gcode, that being said I test ran some basic 3 axis generics cam for a Hass and it worked as it should, for some basic arcs and contour milling a part, I didn’t have the compressor hooked up to the mill so couldn’t do tool changes or check if the cam for them works. Getting a little closer anyway

 

[MaccaRnD]

First basic 3axis g code file, without tool change from SC loaded and works on Masso , for some reason one axis is not moving like it should (out of calibration, moves the wrong distance), I’ll hopefully have time tonight to calibrate the Y axis, really wishing I had a probe and tool setter on tie machine

 

[MaccaRnD]

I’ve recalibrated the Axis and it’s now moving as it should, but I’m having an issue with what I think might be a post processor problem, it’s not machining arcs correctly, so I’m thinking that the post is generating the wrong commands, if there are two consecutive curves it produces the second curve correctly but goes wide on the first curve if that makes sense, it’s not referencing itself or its pivot correctly would be my thoughts. Attached is a picture of what it’s doing top drawing being the expected profile, bottom pic is the weird one with the straight sections sorry the picture isn’t the best the parts rather small amd I couldn’t get a good shot to hi-light the problem.

 

[MaccaRnD]

That’s the code, is there any noticeable errors, the corners are 5mm radius,