Machsupport Forum

Mach Discussion => Mach4 General Discussion => Topic started by: j2mariashop on April 14, 2020, 11:39:31 AM

Title: Mach4 in Fusion 360 Post Processor
Post by: j2mariashop on April 14, 2020, 11:39:31 AM

I create my design in Fusion360 and then use the Manufacture environment to specify the machining operations. Once done, I click the Post Process tab in Fusion 360 Manufacture. In the Post Configuration pull down, Under Vendors I select Artsoft, and Milling. However, the pull down options then available are only Mach2 Mill and Mach 3 Mill. I have to go to the Autodesk HSM Library and download a Mach4 post processor into my local drive, and then upload into Fusion360's post processor. Why is Mach4 not an available option in the pull down menu?

Joe

Title: Re: Mach4 in Fusion 360 Post Processor
Post by: Bill_O on April 14, 2020, 03:04:23 PM

Because the same file you would use for Mach3 you can use for Mach4.

Title: Re: Mach4 in Fusion 360 Post Processor
Post by: smurph on April 16, 2020, 01:53:54 PM

Actually, Mach4 is compatible with most Fanuc post processors that support Tool Compensation Memory Type C Fanucs.  A Fanuc 21i is an example.  We did this by design to eliminate anyone ever having to have a post processor expressly written for Mach4. 

Mach3 had some differences from Fanuc that required its own post processor.  However, For a mill, Mach3 and Mach4 are pretty compatible, G code wise.  Mach4 is more strict about how the G code is written than Mach3, so your mileage may vary when trying to use a poorly written Mach3 post processor that doesn't implement canned cycles very well.  I have no idea if the Fusion 360 Mach3 post processor falls into this category. 

The main differences are between Mach4 and Mach3 are in the Lathe interpreter.  Mach3 lathe G code will most likely not work at all in Mach4. 

So if you want to avoid running into any of those type of issues, use a Fanuc post processor. 

Steve

Title: Re: Mach4 in Fusion 360 Post Processor
Post by: Stuart on April 17, 2020, 04:18:04 AM

Here is the answer go to
https://cam.autodesk.com/hsmposts?

Vendor drop down select artsoft

Or just search for Mach 4 mill

There ye will find the pot of gold at the end of the rainbow

Just copy to your local post lib or upload it to the assets in f360 cam post and select cloud posts from the pp drop down

Title: Re: Mach4 in Fusion 360 Post Processor
Post by: RecceDG on April 28, 2020, 09:51:20 AM

Note that the current Mach 4 Lathe postprocessor on HSMPosts doesn't support Mist coolant.

Title: Re: Mach4 in Fusion 360 Post Processor
Post by: Cbyrdtopper on April 29, 2020, 09:34:28 AM

RecceDG
Here is a post processor that I edited to use Mist.
Be aware this post will also give you the option to use a mist collector, you will see it in the post properties.  It will output "m115" at the beginning of a program and will output "m116" at the end of a program is enabled.