OUPLAN With Automatic Tools Post Processor - Github Sharing

[x3msnake]

Greetings

I Have made for my own use a PP for the Portuguese Brand  of CNC machines Ouplan.

It is published and shared it in my github 

https://github.com/X3msnake/Ouplan-CNC-Fusion-360-Post-Processor

Best Regards

V.

[al.whatmough]

Nice work.  Do you want us to add this to the library of Stock post?

[x3msnake]

Sure, why not 🙂

--
Com os melhores cumprimentos,
Vinicius Silva

[Anonymous]

Very good 😉 Will it work with an Ouplan 3020?

[x3msnake]

yes, probably out of the box

--
Com os melhores cumprimentos,
Vinicius Silva

[Anonymous]

Nice.. I'll give it a try tomorrow.

Btw.. I think we've met in Fabrica Moderna last month 😉

[x3msnake]

Yeah i though it was you 🙂

Hope it is usefull

Drop me a msg here with the results of your testing

[Anonymous]

Hey Vinicius.. 

Everything is working 😉 thanks

Just have one issue but i think it's software related. When creating the NC file, it gives an error about the WCS and uses G53 instead of G54. I've been manually correcting this but is there a way to fix this?

Thanks again

Dave

[x3msnake]

That's not an error

It is a feature. It warns the user what wcs is selected, since you can use any of the machine's available Coordinates (G54-G59) for machining by setting it up in your inocam's jog panel .

In the wcs setup you must use wcs offset 1 or higher.

Anyways the script was designed to default to G54 if the user forgot to set the right offset so there is some issue there. 

Can you share with me a cam setup that you have that is giving you that issue?

[x3msnake]

I've updated the post on Git to fix the WCS validation issue

Now when a user forgets to change the WCS in setup>postprocessor>wcsoffset it defaults posting to G54 and alerts the user of this

[Anonymous]

Sorry, it was my day off, i couldn't check that. 

Tomorrow i'll send you the settings and a copy of the start and end of the gcode where i had to change. I'll give it a try with the new update 😉

Thanks again

[Anonymous]

So part of my problem i'm pretty sure is due to the fact that the network and user permissions don't allow Fusion to run properly. It gives an error saying "Fusion is unable to install Brackets due to unkown error" when i try to access the post-processor configuration menu. 

The gcode now starts with G54 by default but remains G53 in the end.

%
:1248
(Made in : Autodesk CAM Post Processor)
(G Code optimized for Ouplan 2515 with InoControl controller)

(Program Name : teste2)
(1 Operation :)
(1 : Morphed Spiral2)
(  Work Coordinate System : G53)
(  Tool 8 :Flat End Mill 2 Flutes, Diam = 4mm, Len = 13mm)
(  Spindle : RPM = 15000)
(  Machining time : 1 min 27 sec)

G40 G17 G80 G49 G21

(Operation 1 of 1 : Morphed Spiral2)

G90 G54
G0 X0 Y0

T8 M6 M9 M3 S15000
G0 X0.308 Y0.308 Z15
G0 Z-1.064
G1 X0.308 Y0.308 Z-2.641 F1000
X0.216 Y0.216 Z-2.936

(...)
(...)

X34.459 Y30.328
G2 X34.788 Y29.595 I-0.792 J-0.796
G1 X34.796 Y27.784
X35 Y-30
X35.001 Y-30.283 Z-22.355
Y-30.4 Z-22.072
G0 Z15

M9
G53 G0 Z150
G53 G0 X20 Y20
M30
%

I'll have to check on my laptop if i can change the configurations and the problem goes away, but apart from that, everything is ok 😉

Thanks again

[x3msnake]

Greetings Master

What do you need from me in order to add this post to the library?

[x3msnake]

The last move is intentionally in machine coordinates,

You want the machine to go to a safe and know position before it ends the program.

It is intended as a back to base setting you can set your own final spot by changing the user settings in the post screen

As for the brackets as long as you untick the open NC file in editor it will not try to install brackets

[x3msnake]

New Update

User  now has the ability to disable ATC for machines with disabled tool warehouse

With the option set to false it will default any tool to T1 to avoid spindle plunge caused by undefined tool offset

// If the user defines his machine as having no ATC > Set default tool to T1
    if (properties.hasAutomaticToolChange)
        {
        var validateToolNumber = tool.number;
        } 
    else
        {
        var validateToolNumber = 1;
        }

	if (isFirstSection()||(tool.number != getPreviousSection().getTool().number)) // Skipping posting instructions when the new operation is using the same tool number
	{
		writeBlock(tFormat.format(validateToolNumber), mFormat.format(6), mFormat.format(table_vacum), mFormat.format(tool_direction),sOutput.format(tool.spindleRPM));
	}

https://github.com/X3msnake/Ouplan-CNC-Fusion-360-Post-Processor/blob/master/ouplan.cps