Frage Fusion 360 Post Processor Attached in Here

Hi Guys,

I can see a number of people are requesting a Fusion Post that works with Stepcraft.

I have attached the latest one I have, that is setup to be able to use the Stepcraft with or without the 4th "A" axis.

Some notes about how to ensure your CAM operation works
1. The Pass tolerance in the FUSION360 CAM operation "pass" menu MUST NOT be left at .001mm, you need to increase it or else you will have an ARC error when you load the part in the UCCNC program. You need to set this each time you create a CAM operation when you check what parameters you have, and I increased it to 0.02mm without issues, if you see tolerance listed anywhere in fusion, it cannot stay at .001mm!

2. The CPS file attached, has the 4th axis enabled, which just means, if you create a single setup, and say two operations, If the second operation you click on the second menu, tool orientation, and move the Z axis to where you want the tool to come down from ( ensuring the Y and X axis are correctly assigned as if the part is rotated in the 4th axis ) , then highlight both completed operations and ask for a Post.... In the post, between the two operations, there will be an A command, which is A axis. Once the Post has completed, view the post and search for A. Above the A command, look at the last position for X/Y/Z, as this is where the tool will be, when the 4th axis is rotating to the new position, which you may want to manually change depending on what you are rotation on the A axis, Ie maybe move X left by 200, rotate, and then let the head continue with the passes.

I always view the A commands before they occur, and at the end of the last one, to make sure the machine isn't doing stupid stuff positioning wise. I normally run with soft limits off, as we use the center of the rotation axis as the Z=0 value as it is simple to place a sketch point in the center of your stock to select as the origin for z=0

We also disabled the first of the G28 commands as it would sometimes change our offsets, and go to the wrong part of the machine to machine parts. Insteadd we manually zero'd x/y/z where we wanted them, clicked home all, normally moved the toll close to start point ( in that direction ) then clicked play

You can just put this post processor in a file anywhere, an in fusion, Post, click config file,m and Open from, and point Fusion to the folder, then you will be able to select this file from the option menu,

Nick

Enjoy

YOU MUST RENAME THIS FILE TO .CPS instead of.TXT as this forum will not let me attach at.cps !!!!!!!!!! WTF





Why isn't my attachment appearing here ?

My post is from auto desk.

It was a genetic mach3 file, which I modified to enable 4th axis. The tolerance is still an issue, if it is set too low, uccnc gives arc error.

Hi all,

together with Stepcraft we have made a specific uccnc post processor for stepcraft machines which is available here:
https://forums.autodesk.com/t5/hsm-ideas/generic-stepcraft-uccnc-post-processor/idi-p/6510523
http://cam.autodesk.com/posts/?p=stepcraft_uccnc

Note that there are properties for G53 positions to be able to set a tool change position.
Also you have the option to activate your fourth axis (which can be mounted along X or Y).

It would be great if you could provide some feedback so that we can release it as soon as possible.

@finch,
You said you had issues with arcs?

"1. The Pass tolerance in the FUSION360 CAM operation "pass" menu MUST NOT be left at .001mm, you need to increase it or else you will have an ARC error when you load the part in the UCCNC program. You need to set this each time you create a CAM operation when you check what parameters you have, and I increased it to 0.02mm without issues, if you see tolerance listed anywhere in fusion, it cannot stay at .001mm!"

[/i]

I cannot reproduce this issue on any part on my UCCNC, could you please share your part + the nc program?

Hi AutodeskCAM Posts,

is there a plan to have WinPCNC postprocessor in near future?
Stepcraft started with WinPCNC, so many Stepcraft users use this software.


Thanks,
Marco

Coming soon

Many thanks.

Hi,

I’m successfully using Fusion 360, but when I post a NC file using the Autodesk postprocessor for Stepcraft/UCCNC it adds G28 toward the end of the program. If I don’t remove this command (move to home position) I get an error message if I try to run the program. The attached jpg shows the message. It seems like UCCNC believes that the home position is outside of the soft limits for UCCNC although I’ve zeroed all axes well inside the the machine coordinate system. I’m starting to belive that this is bug relating to a mixup between the machine coordinate system and the work coordinate system.

Can anybody confirm whether this is a bug or have I missunderstood something?

Warmly, Per Takman

That issue is already under investigation by UCCNC.
We have updated the post processor to avoid these problems regarding this.
The post is available here:
cam.autodesk.com/posts/?p=stepcraft_uccnc

Thank you! I discovered this while searching for further information on how to modify the post processor myself. The new pp works very nicely.

I have two additional feature requests for the pp:

1. Support for compensation of skew between x- and y-axis. I have not found any support for this built into UCCNC, but I've requested more information from cncdrives.com.

2. I've found that the quality of the cuts made with the Stepcraft drag knife when used with vinyl improve a lot when adding fillets to internal corners where the angle of the corner is below some threshold value. It would be great if the pp could add this for me. Preferably using a true/false and a radius setting and why not do the same option also for external corners in cases where robustness of the decal is of importance.

Any help towards achieving this would be fantastic, because I have not figured out yet how to rewrite the pp myself yet.

Warmly,

Per Takman

1) out of square?

the way to solve is not by post processor... by hardware. adjust the two gantry sides? this would be very tricky with the post - its geometry.

2)

Sheet CAM has some good feature recognition features that let you identify certain aspects of a toolpath
vcarve has fillet tool so you can do it manually.

1) is more a hardware thing
2) have a look into the passes tab and look for "Minimum Cutting Radius" or "Finishing Smoothing Deviation"
http://help.autodesk.com/view/INVHSM/2015/ENU/?guid=GUID-CBDA3AF7-E0D9-4861-9D7D-6A543EC2D4AF

Thanks Rory,

1. I know it is better to solve it mechanically whenever possible, but I'm expecting that I will have difficulties adjusting one y-axis screw relative to the other if it comes down to making single tooth adjustments on the belt drive. Maybe you have some good tricks to share with us?

2. I'm looking for a way to do it in Fusion 360 automatically since it is free for hobbyists and I'm starting to like it. It seems like it should be doable, but if the Autodesk crew are willing to assist it would surely speed things up for me at least.

Cheers,

Per

Thank you for the suggestion!

It almost does what I want, but from what I understand it will add a radius regardless of whether the corner is internal/external and whether the corner is pointy or blunt. I want to control behavior based on these criteria, which requires some kind analysis of the geometry.

Until I find a way to automate this I think adding a radius to the model is the only way to achieve the selectivity I want.

Cheers,

Per

Close,
minimum cutting radius will add the specified value to internal corners if it would result into a sharp corner.
eg:
Tool Diamter D4
Corner radius R2
would result into a sharp corner into the toolpath.

Tool Diameter D4
Corner radius R2
Minimum Cutting Radius 0.5
would result in a toolpath where without sharp corners by adding 0,5 to the toolpath into this area.

So it depends on your tool diameter and the geometry.

I see... maybe it will solve my problem then. Thanks for clarifying.

/Per

Thank you for the suggestion to use minimum cutting radius!

I changed the drag knife "diameter" to 50 µm and set the minimum cutting radius to 24 µm. I also had to set the number of stepovers to 0 in order only get one single pass with the knife.

The result was very satisfying with virtually no overcutting in sharp pointy inside corners, but still very sharp outer corners.

Problem solved!

Cheers, Per

Cool, thanks for your feedback!

For all users waiting for a WinPC-NC post processor... As promised, here it is:
https://cam.autodesk.com/posts/?p=stepcraft_winpc-nc