Fusion 360 on Y axis lathes

[AdamsCNC]

Hi,

We are thinking of buying Fusion 360. We have a series of holes and threaded hole to machine on a flange. Is fusion capable of posting to lathes with a Y axis and does it actually work?! I am a experienced HyperMill programmmer, however my current company this software is overkill for us.

Regards,

R

 

[Chips Everywhere]

Ran a Haas with a sub spindle and Y axis, you can use Fusion360 for it, but you will more than likely need to end up editing a post processor to meet your needs, the one that Fusion provided was crap at best. I believe they will give you your money back within 30 days if not happy. Also, Fusion loves to do updates, sometimes these updates will throw a monkey wrench into your whole set up.

 

[AdamsCNC]

Ran a Haas with a sub spindle and Y axis, you can use Fusion360 for it, but you will more than likely need to end up editing a post processor to meet your needs, the one that Fusion provided was crap at best. I believe they will give you your money back within 30 days if not happy. Also, Fusion loves to do updates, sometimes these updates will throw a monkey wrench into your whole set up.

Thanks mate appreciate your comments. If it can give me the meat of the code thats all I am after! I could use some software I already have for mills, issue is on a lathe X is a diameter figure so this means it will not work on my lathe

 

[Chips Everywhere]

Good luck, it can be done, just double check yourself to avoid a crash

 

[Liberty_Machine]

Yep, relatively easily done. I have a Doosan Lynx LSY and use Fusion regularly for it. I've tweaked the post processor a fair bit, as I'm somewhat anal about code formatting.

 

[EricTheLatheGuy]

In my opinion, fusion 360 is good enough to make both X+C axis and X+Y+C axis live tooling programs. Running a DMG MORI with fanuc 32i-ihmi control, and so far, for the few programs I had to make with a CAM software, it was great!
Our programmer uses mastercam, wich have exactly the same post processors, and being the one that runs the machine, I have to say, when you know what codes your machine wants and needs, you are well placed to work on thoses post processors. F360 should do the job. Good luck!

 

[Rayond]

Yep, relatively easily done. I have a Doosan Lynx LSY and use Fusion regularly for it. I've tweaked the post processor a fair bit, as I'm somewhat anal about code formatting.

Hi there, would you be so kind to help us a bit with a Fusion360 post processor for LYNX 2100LSYB? We are using the generic postproc from Doosan for LYNX/PUMA, but it needs some adjustments to work properly. Can you please guide us where to start? Is there any editor for the postrproc? Thanks a lot!

 

[Liberty_Machine]

Hi there, would you be so kind to help us a bit with a Fusion360 post processor for LYNX 2100LSYB? We are using the generic postproc from Doosan for LYNX/PUMA, but it needs some adjustments to work properly. Can you please guide us where to start? Is there any editor for the postrproc? Thanks a lot!

Hmm, the post should pretty well sorted by now. What exactly are you running into for issues? One of my customers just picked up a Lynx 2100 and he's using the generic post directly from Fusion. I'm using a lightly modified version (just light formatting) and that is working properly.

 

[Rayond]

Hmm, the post should pretty well sorted by now. What exactly are you running into for issues? One of my customers just picked up a Lynx 2100 and he's using the generic post directly from Fusion. I'm using a lightly modified version (just light formatting) and that is working properly.

Well, we are using the postproc downloaded from Autodesk - generic Doosan PUMA/LYNX, we have small issues, e.g. the NC code gives us P12 for sub spindle, where P12 should be used for the live tool.. Also, we are using FANUC coding "B" (Europe) in stead of "A" (USA) which has a bit different syntax, e.g. G50 is RPM limit in EU code and threading cycle in US code. There seems to be no chance to edit this in the Fusion Postproc edit environment. Any idea how your customers solved this issue? Again, I really appreciate your help.

 

[Liberty_Machine]

Well, we're US based, so I can't speak to the Fanuc "B". That said, are you selecting the proper machine in the post? There are options for Puma, Lynx, Lynx w/Y axis. That will change which spindles are labeled with what.
I know Autodesk has their own Lynx in their Birmingham Tech Center (UK) and, as far as I know, they're running code straight from the post. (I speak to those folks daily).

 

[escapethewrmhole]

Well, we are using the postproc downloaded from Autodesk - generic Doosan PUMA/LYNX, we have small issues, e.g. the NC code gives us P12 for sub spindle, where P12 should be used for the live tool.. Also, we are using FANUC coding "B" (Europe) in stead of "A" (USA) which has a bit different syntax, e.g. G50 is RPM limit in EU code and threading cycle in US code. There seems to be no chance to edit this in the Fusion Postproc edit environment. Any idea how your customers solved this issue? Again, I really appreciate your help.

I don't think this is correct.
G50 is RPM limit on my Fanucs in NA.
Threading cycles are G32, G76, and G92

 

[Liberty_Machine]

Well, we are using the postproc downloaded from Autodesk - generic Doosan PUMA/LYNX, we have small issues, e.g. the NC code gives us P12 for sub spindle, where P12 should be used for the live tool.. Also, we are using FANUC coding "B" (Europe) in stead of "A" (USA) which has a bit different syntax, e.g. G50 is RPM limit in EU code and threading cycle in US code. There seems to be no chance to edit this in the Fusion Postproc edit environment. Any idea how your customers solved this issue? Again, I really appreciate your help.

I just posted out some code with the OEM post and I'm getting P12 for live tool and P13 for sub spindle. Make sure you've set the machine correctly in the Configuration dropdown, see photo.

 

[Rayond]

I just posted out some code with the OEM post and I'm getting P12 for live tool and P13 for sub spindle. Make sure you've set the machine correctly in the Configuration dropdown, see photo.View attachment 429497

We have selected the correct machine, as you described, however I still get P22 for live tool, which I really don't understand, and P11 for sub-spindle. Regarding the US coding (G50 for RPM limit) - I can live with that, but this spindle and live tool mismatch is a real pain, as you can imagine.

 

[Liberty_Machine]

I'm going to drop you a private message

 

[Liberty_Machine]

Oh, and for your Tool offsets, everything is set to Turret zero:

 

[Rayond]

Oh yes that is pretty important point, we did this wrong. Just figured out our BIGGEST mistake - we did not mark the SECONDARY SPINDLE in the "SETUP" options. Tomorrow I will run some test program on the machine, but I am pretty confident it will work. Once again it was a huge help that you provided.