Post processor for FangLing F2100B

[Anonymous]

I've bought a CNC plasma machine that uses a FangLing F2100B. I'm currently using FastCam to convert the DXF files to NC/TXT files. I'm looking for a postprocessor for Fusion360. 

Is there a standard postprocessor  available??

[Marco.Takx]

Hi @Anonymous,

Go to this website and search for DXF

https://cam.autodesk.com/hsmposts? 

Give it a try.

If my post answers your question Please use Accept as Solution & Kudos This helps everyone find answers more quickly!

[Anonymous]

it realy works for FangLing F2100B?

[govinda_webster]

Hi,

Can you give some more infomation on these processors please? I would really like to forgo FastCam and use Fusion 360 to export straight to our machine. . .

Any and all help apprieciated. . .

Thanks

[Anonymous]

Did you solve this?

How do you currently convert from fusion360 to the fangling F2100B?

[timjames02]

Did you find a post processor that works for the fangling controller??

[Anonymous]

We are still using FastCAM because non off the postprocessors in Fusion360 works for the FangLing CNC.

We have tried various processors, but there's always something that doesn't work properly.  

[jamesnjhelms]

Old topic but it might help someone.

This controller will only read .CNC .NC or .TXT

Use Hypertherm jet in post and set pierce time to 0. Use the pierce time set in your controller.

This controller can read G4 F1 (dwell for 1 second) and set the feed rate to 1mm/m.

Use the default "in computer" kerf compensation within fusion and you're good to go.

If you want to use "in control" kerf compensation then you will need to edit your output code so the G41 command is a line above the M7 (torch on) otherwise it will pierce and pause or do a double pierce.

If you want to use the controllers speed settings on the fly then you can delete the F command from your program. The F will override anything you have set in the controller.

None of this following stuff is necessary but it helps to keep things simple.

In post preferences you can turn off "use sequence numbers" "write machine" and "allow head switches"

If you want you can delete the M19 and M30 at the end of your program, though the machine will ignore them anyway. The correct command to end program for this controller is M02 or M2 though it will just end with no problem if there is no more code to read.

[mspecdesign]

thanks, ill give this a go today!

update: confirmed this worked fine, thanks jamesnjhelms

side note: The usb stick must be formatted to fat32 for the F2100b to read it.....had me frustrated for a bit that one haha.

[jamesnjhelms]

Happy to help, thanks for the feedback.

Yeah the USB drive must be fat32 and there is also a capacity limit (16GB or 32GB?)

I have at least one fat32 USB drive that the machine refuses.

It's not a bad controller, in fact I really like it. I have ours setup with plasma and an LPG torch and it's done a ton of work, including full 2.4m x 1.2m nests, thousands of lines of code. Once you have your kerf dialed in it's as accurate as any, so long as your stepper motor pulses are dialed in (to do this, sharpen a tungsten or a piece of wire or similar and tape it to the torch holder, then run a tape measure down the X and Y and use the step function "step move" set to something big, like 2400mm or what have you. Adjust motor pulse until it's perfect)

I have since edited hypertherm's post processor to further suit this controller. Output code looks like a native "shape library" program and requires 0 editing, but it only works with the default "in computer" kerf settings in fusion.

I have a separate file for "in control" kerf settings if you're hell bent on setting kerf values from the controller (ask if needed)

[baabafadil]

Thanks for the Tips though request you do like a video tutorial & post on YouTube & give us link here thanks 

[ajmetalwork]

Hi James,

Just wanted to say thank you for posting this!!

You have saved me hours of time trying to set this up

THANK YOU!!

[mdominguezNEMWY]

Tnx for the cps, it works wonderfully!!!