Calypso water jet post

[Anonymous]

Hi all.

I need to find a post for a Calypso water jet. 

apparently this machine uses NC GeoMate http://multicam.ca/nc-geomate-software-for-waterjet/

to automatically create its own cut program and basically you feed it a dxf and it does the rest. 

how ever we have tried supplying the sub contractors with a dxf created by fusion! but no luck in the DXF export from fusion being able to translate into the sub contractors cad package. 

Now I don't know if this yet another fault of the fusion sketch engine! But I need to get these bits cut like last week! 

So the solution was to try and output a program from fusion! 

I can't find a way of outputting a program! 

Has anyone got experience of the above water jet! is there a post that will work! 

Apparently a Multicam post should work but all i get is this! 

As you can see. drawing a bit of a blank here! 

Some help would be greatly received! 

Information: Configuration: MultiCam ISO

Information: Vendor: MultiCam
Information: Posting intermediate data to '/Users/user/Desktop/1.cnc'
Error: Failed to post process. See below for details.
...
Start time: Fri Nov 4 12:24:42 2016
Loading locale from '/Users/user/Library/Application Support/Autodesk/webdeploy/production/8beef08b232ffde48d2a02741cfc403a7f8753bf/Libraries/Applications/CAM360/Data/Posts/common.en.lang'
Post processor engine: 4.2.1 40927
Configuration path: /Users/user/Library/Application Support/Autodesk/webdeploy/production/8beef08b232ffde48d2a02741cfc403a7f8753bf/Libraries/Applications/CAM360/Data/Posts/multicam.cps
Include paths: /Users/user/Library/Application Support/Autodesk/webdeploy/production/8beef08b232ffde48d2a02741cfc403a7f8753bf/Libraries/Applications/CAM360/Data/Posts
Configuration modification date: Tue Jun 28 18:25:16 2016
Output path: /Users/user/Desktop/1.cnc
Checksum of intermediate NC data: 792163fdc412e17c9a9338c5ad774598
Checksum of configuration: 0e96fc9f0343f93880459a76af0c7233
Vendor url: http://www.multicam.com
Legal: Copyright (C) 2012-2016 by Autodesk, Inc.
Generated by: Fusion 360 CAM 2.0.2455
...
Error: Waterjet, laser, and plasma cutting toolpath is not supported by the post configuration.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to invoke 'onOpen' in the post configuration.
Error:
Error: Failed to execute configuration.

[xander.luciano]

Hey there!

You said the software "automatically create its own cut program and basically you feed it a dxf." So you are looking to export a DXF of the toolpath, however you used a Milling Post processor which creates gcode. I would recommend downloading the DXF post processor from here: http://cam.autodesk.com/posts/?p=dxf

Save it to C:\Users\YOUR USER\AppData\Roaming\Autodesk\Fusion 360 CAM\Posts
or somewhere else.. just DO NOT save it with the generic posts.

For you waterjet operation, you can leave the tool tab at it's default settings (waterjet cutting, through -  auto, .08 kerf, etc.). Select the geometry/edges/contours you want to export to be cut, heights can be default as well (we're going to discard all that data when we export to DXF anyways), then go to the passes tab and change the compensation to center instead of left.



This prevents it from applying the kerf offset to the part since the other software will account for the offset.

Lastly, under the passes tab, disable lead in and out so those don't get included in the DXF file (just uncheck the boxes.)

Now post your operation and choose "Personal Folder" to load up your personal posts



Lastly, change the "onlyCutting" option to Yes so that only the toolpath is output to the DXF file since the other program will create the linking movements. Save to wherever you please and enjoy your Autocad DXF.



If that doesn't work you can try using the Universal Laser DXF post processor instead, but you'll need to change the operation to be laser instead of waterjet.

Let me know if that works!
Good luck on the parts,
Xander Luciano

[daniel_lyall]

@Anonymous the other option is there is a plugin for exporting .dxf files here for lasers but it can be use to just export a .dxf https://apps.autodesk.com/FUSION/en/Detail/Index?id=7634902334100976871&appLang=en&os=Win64  it only export one face at a time but it's a very clean .dxf

[xander.luciano]

An even simpler method! I like it. 🙂

[daniel_lyall]

It's a new plugin it's only been there a week or so.