Fanuc lathe Post processor changing M03 to M04

[nrmplastering]

Hi all,

I am just in the process of setting up a new DMTG slant bed lathe fitted with FANUC OiMF control. I have posted a program out with the FANUC PP and all seems fine up to now apart from I need it to post M04 spindle rotation rather than M03 that it is currently doing. I am hoping someone might be able to point me in the direction of how to change this, preferably so I can learn what is being changed rather than someone just doing it. 

Many thanks in advance

neil

[engineguy]

@nrmplastering 

So, are you saying that your Lathe spindle runs Counter Clockwise and the tools are facing upwards in the Turret?

Found a video of the Lathe and it appears to be of standard layout with the Spindle rotating Clockwise and the tools face downwards so the M03 would be corrct for the Lathe layout as far as I can see from the video.

Video Link :-  https://www.youtube.com/watch?v=jkWpH0SkJ8U

[nrmplastering]

My chuck rotation is opposite to this video attached

https://www.youtube.com/watch?v=exdvmHC6Ukc

If I am stood behind the chuck looking into the lathe M4 is CW and M3 is CCW

M4 needs RH tools and M3 LH tools

[engineguy]

@nrmplastering 

OK, if it is the case that your tools are facing upwards on a Slant Bed Lathe then yes, you will need the spindle to run Clockwise as viewed from the front of the chuck, I actually still have a very old Lathe in my shop that has the same configuration, here is an image of the place in the Fanuc Turning Post Processor showing where to change the (3) to a (4) so that the output will be an M4, hope that is of some help, as I don`t have the exact Post Processor that you are using what is shown is only an example but all you need to do is change the (3) to (4) where it is highlighted in the image to make the change.

WARNING !! If you didn`t already know this, whenever Autodesk updates a Post Processor then your change will be lost and the PP will default back to the (3) setting.

You must place the PP in a safe location such as your "Cloud or Local" Post Library and always use it from that location.

Also go to your "Preferences" and turn off the Automatic Post Processor Updates just to be safe, this means that you will not get the latest version of your Post Processor but if what you have works fine for you then stick with it.

[nrmplastering]

Many thanks for your help, it is much appreciated. I have had a look through the Post processor that I have here and can find this information as per the screen grab. Is this the correct location? 

It has both 3 and 4. To reverse the rotations would it be a case of swapping these about, so they are opposite to what they are at present. 

Thanks again

Neil

[engineguy]

@nrmplastering 

As I don`t have a copy of your Post Processor to test with here is what you can do to get the code to be output with an M4 instead of an M3.

This can all be done in Fusion Tool setup rather than Editing/Modifying your PP, have a look at the images below and try doing the same your end, works fine here 🙂

OK, first image is Tool Holder setting, Left or Right, you need Left as below.

Seccond image shows the Tool Setup and you need to uncheck the "Spindle Clockwise Rotation" as in the image below.

The above two settings should give you a configuration as shown in the image below, Tool is facing upwards and the Rotation is CCW as viewed from behind the Spindle and CW as viewed from the front of the Chuck.

The above three images should give you G Code M4 for the Spindle Rotation as in the image below.

Hope the above is of some help to you 🙂 🙂 🙂

[nrmplastering]

@engineguy 

That is a massive help. Thankyou so much, you are a diamond. 

I've had a play about with them setting and it looks like it will give me what I need. I am not at the lathe for a short while so will give it a try and update you when I have got it going. 

Thankyou once again. 

Best wishes

Neil.