My Mill or Their Code?

Hello All,
            I asked a related question a year ago and we got it resolved, but i'd like to know what's actually going on.
            
            Full disclosure I know what G54 is - that's it. With that being said my cnc mill is running great and i'm happy with the success. O'kay, so i'm using fusion 360 and in my post nc files using grbl as the processor i'm getting the following lines
            
            at top (about ten lines down)
            G28 G91 Z0
            G90
            
            at bottom (two tool lines follow before end)
            G28 G91 Z0
            G90
            G28 G91 X0 Y0
            G90
            
            So when these lines run they drive my endmill into the table. Deep. At the beginning it drags through the work to the desired start point, raises and begins the ramp or zigzag descent. It's brutal. So i try to remember to remove this from every file and then most times do a "simulation" in linuxcnc by just not powering on the steppers.
            
            ...anyways... What can I do about this? Is there some machine setup that i missed? I figure if fusion 360 is placing these lines in everyone else's files it must be normal. So what can I do to make my machine do something desirable when these lines are present?
            
            Thank you,
            John

G28 is a pre defined position. Jog your machine to a safe position above the table and enter g28.1 mdi command. This will store that position as the g28 position.

Read the gcode documentation.

Hey Henk,
Thank you! Will this be stored permanently or will it reset when i shut down? edit* it looks like it might be stored. The G28 position is stored with G28.1.*

I have tried reading the documentation. I've always had trouble learning by reading certain things. It just becomes overwhelming and nothing at all sinks in. I hate it.

Thanks again,
John

It might be F360 has a different view to you. It assumes that Z0 is at the top of travel and downward travel is negative.
So G28 G91 Z0 should move to the top of the Z axis (without a G28.1)
Linuxcnc stores all variable data like your G28 setting in a file ending in .var in your config folder between sessions

If I remember correctly it is also possible to use G53 instead of G28. Have a look at the post process screen and I believe you should have the option of G53 or G28 for 'Safe Retracts' (G28 is the default). Then with G53 it should also be possible to set the x y z home position directly within the same screen (just above safe retracts). (<-This is only for turning posts)

Note that this also depends of which version of the post processor you have. I'm sure that v43654 and up have it, while 42049 does not.

Post processor are here: cam.autodesk.com/hsmposts


 

Ohhh   I see that you mentioned that you're using the grbl post processor. I'm not sure you have the same options (G28 or G53) with that...

Why not using the post processor developed specifically for linuxcnc instead?

I found about a year ago that I was supposed to use grbl/grbl processor for linuxcnc. I also found that again recently as i had forgotten. What processor should i be using? 3 axis cnc mill.

Thanks,
John

Bumbino wrote:

I found about a year ago that I was supposed to use grbl/grbl processor for linuxcnc. I also found that again recently as i had forgotten. What processor should i be using? 3 axis cnc mill.

Thanks,
John
 

Well, I guess you can use whatever suits your machine BUT I don't see any reason why the Autodesk HSM post for Linuxcnc mill would not work with Linuxcnc mill. Then I've also checked that the latest version of grbl post also allow you to choose G53 or G28.  

My suggestion would be to first try selecting G53 with your current grbl post processor and see if that correct the problem the way you want your machine to work. If not then it is just a matter of downloading the LinuxCnc post, install it and select it when you process it. You can this way easily switch posts to compare the file generated by both.

The other thing is that you must also have the minimum required 'post engine version'.for a given post. This is not a problem if you have the latest Fusion 360 (2023) but if not fusion may fail when processing the files. Have a look here: forums.autodesk.com/t5/hsm-post-processo...update/td-p/10182498  Not linuxCnc but related same way.

 

Good writing about G28 vs G53: www.mmsonline.com/articles/g28-versus-g53