Tool Home Position (Lathe)

[StevenL]

I successfully completed a class in MasterCAM as I picked up a position to allow a business to bring in work to their own CNC lathes.  I talked them into purchasing MasterCAM for SolidWorks and I was pretty much on the hook to make it work.  Up until now their machinist would manually enter parts via the control panel and play with arcs and flats to get a part machined.  It was pretty tedious to do.

I was able to quickly design parts in SolidWorks and model tools and create programs from the desktop computer.  Now I carry a thumb drive to the CNC lathe and give them the tool setup and stock sizes and they start production parts as is.  It's great.

Now we have a second new HAAS machine (our first HAAS) and I've got the new Post Processor files and I have been able to run simulations with a new Machine Group, but there's this perplexing issues of Tool Home Position.  I basically manually enter the home position values on the first machine into each tool and it seems to work.

Here's the question:  What exactly is the Home position?  I believe it's the place the turret goes to change tools.  It can be User Defined, Tool, or Machine based.  I read the X and Z position off the machine when at home and I used these numbers.  Is this the way to go or can I use the values pre-set in MasterCAM?   I believe it's Machine is default  (X:5. Z:10), Tool (what ever I programmed into the tool model).  

I know this should be simple but at this time clarity would be good. 

Steve

 

[Colin Gilchrist]

3 hours ago, StevenL said:

I successfully completed a class in MasterCAM as I picked up a position to allow a business to bring in work to their own CNC lathes.  I talked them into purchasing MasterCAM for SolidWorks and I was pretty much on the hook to make it work.  Up until now their machinist would manually enter parts via the control panel and play with arcs and flats to get a part machined.  It was pretty tedious to do.

I was able to quickly design parts in SolidWorks and model tools and create programs from the desktop computer.  Now I carry a thumb drive to the CNC lathe and give them the tool setup and stock sizes and they start production parts as is.  It's great.

Now we have a second new HAAS machine (our first HAAS) and I've got the new Post Processor files and I have been able to run simulations with a new Machine Group, but there's this perplexing issues of Tool Home Position.  I basically manually enter the home position values on the first machine into each tool and it seems to work.

Here's the question:  What exactly is the Home position?  I believe it's the place the turret goes to change tools.  It can be User Defined, Tool, or Machine based.  I read the X and Z position off the machine when at home and I used these numbers.  Is this the way to go or can I use the values pre-set in MasterCAM?   I believe it's Machine is default  (X:5. Z:10), Tool (what ever I programmed into the tool model).  

I know this should be simple but at this time clarity would be good. 

Steve

 

This is exactly the place where the Turret goes "home" to change tools.

What "home" means, will depend, based on your Post Processor configuration & based on your Parameter settings in "Miscellaneous Values" in the Operation.

This is the "Misc. Values" button in your Picture.

The "Misc. Values" are Integers and Decimal (real) numbers, that act as "input" to the Post Processor.

With many Lathe Posts, the value of 'mi1$' will configure the output of Tool Change (home position) output.

Here is the Commented Text, from the top of MPFAN.PST:

# mi1 - Work coordinate system: (home_type)
#       -1 = Reference return / Tool offset positioning.
#       0 = G50 with the X and Z home positions.
#       1 = X and Z home positions.
#       2 = WCS of G54, G55.... based on Mastercam settings.
#
# mi2 - Absolute or Incremental positioning at top level
#       0 = absolute
#       1 = incremental
#
# mi3 - Select G28 or G30 reference point return:
#       0 = G28, 1 = G30
#
# mi4 - Canned conversion cycle type selection:
#       Mill-
#       Activates milling axis conversation canned cycles (G107 or G112).
#       1 or -1 activates the cycle, the path continues until next entry is
#       zero, sign switches (1 to -1) forces g113 at null toolchnge, the
#       cycle changes or the tool changes.

 

[Colin Gilchrist]

I think the thing to note here is this:

You don't "have to" go all the way back to the Machine Home Position, when changing tools. It always depends on the individual machine and the part you are programming.

Also, it really depends on the Method that was used to setup the Tool Offsets, and if you are using a Work Offset, or not.

This can all be super confusing for a new programmer, because there are just "so many different options"!

What is right? Well, whatever works for your particular shop and people, is the right way to do it.

Many of the "old school" Methods that people use, were based on "options" that were available on the controls at the time.

Most "new" machines have more advanced options available, so the Methods that are used on the new machines might be completely different from what you did on the older models.

This might help you:

https://www.haascnc.com/content/dam/haascnc/en/service/manual/supplement/english---chucker-lathe-operator's-manual-supplement---2020.pdf

https://www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---lathe-ngc---operator's-manual---2020.pdf

https://www.haascnc.com/content/dam/haascnc/en/service/manual/supplement/english---toolroom-lathe-operator's-manual-supplement--2020.pdf

https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/lathe---programming-workbook.pdf

https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/lathe---programming-workbook---answers-book.pdf

https://www.haascnc.com/content/dam/haascnc/en/service/reference/programming-workbooks/shop-notes---machinist's-cnc-reference-guide.pdf

https://www.haascnc.com/service/troubleshooting-and-how-to/reference-documents/spindle-liner-kit-reference-table---ad0022.html

https://www.haascnc.com/video/tipoftheday/lfgsp9mtzqg.html

https://www.haascnc.com/video/tipoftheday/x24u0exmltk.html

https://www.haascnc.com/service/troubleshooting-and-how-to/reference-documents/part-catcher-macro-program--m36-parts-catcher-close-.html

https://www.haascnc.com/video/tipoftheday/G6vHC9Z1eBs.html

 

 

 

[Mavyhui]

 

pcan1, pbld, n$, *sgcode, *xh$, *zh$, e$