haas tm1 toolroom mill post processor ?

[mogtract]

Hi folks

I have access to a haas tm1 cnc toolroom mill milling machine, but no access to cad cam software. (mill is currently being used with its own "visual quick code" and manually)

Having found cambam i was hoping my probs. had been solved, and could do a few more advanced projects.
I created the "stepper motor mounting plate" with the tutorial and now want to try it out on the machine.

But :

1. Which post processor do i choose in the drop down machining menu? I have a very limited understanding of cnc ing and even less of cad cam

2. once i choose the correct post processor how do i get the "gcode" onto a usb stick to take to the above machine?

I tried doing a search but couldnt find anything.

I look forward to any advice

Many Thanks

Mogtract

[10bulls]

Haas should be compatible with a Fanuc post.
There are two Fanuc post processors provided, however, to get them working for your specific machine, I would recommend getting a basic understanding of the post processor files.
http://www.cambam.info/doc/plus/cam/PostProcessor.aspx

The standard Fanuc post (Fanuc.cbpp) contains % % characters which are for serial transmission, so you would need to remove these for copying via memory stick.

The Fanuc DK post was kindly provided by a CamBam user and was specific to the Mori Seiki he is using.  It does not have the % % delimiters, but does have some extra tool change and return to home commands.

As to question 2... you would generate a g-code file from with CamBam as per the tutorials, then simply copy this to the memory stick.  The g-code file might need a special extension for the Haas to recognise it.

Sorry if all this sounds a bit vague.  I've not used a Haas myself.
(I'm hoping someone with a bit more Haas experience may pitch it  )

My limited understanding is that the "visual quick code" you describe can also be saved to a usb stick.
If this is g-code like, then if you can upload a file generated by the Haas, it may give us enough information to help you put together a sensible post processor file.

I hope this helps and good luck!

[10bulls]

Update!
It sounds like I made a couple of boo-boos in my previous advice! 

I've just spoken to a friend who teaches CNC at college where they use Haas TM1s.

Apparently you DO need the % % delimiter characters, when loading g-code from a memory stick.
You also need a program address O##### as the first command after the %.
That is capital O followed by a five digit number.
The Fanuc.cbpp post processor should be pretty close to this.

The Fanuc.cbpp post processor contains a user defined macro {$o} for the program address.
This needs to be defined in the PostProcessorMacros property (under the properties when selecting the Machining folder) of your CamBam file.

For example
$o=00123

I'm not sure if there are valid program address ranges you need to use, but presumably you need to check that the address you specify is not already in use.

I would stress again though, I am not experienced with Haas machines.  I will happily advise you on how to modify a post processor to suit your machine, but you should double check that the resulting g-code is suitable.

[mogtract]

Hi there,

Thanks for the reply 10bulls and for asking your teacher friend.

 I downloaded the cambam post processor files as suggested and have been reading through them.  I haven’t fully grasped the lingo yet. ( I’m not the sharpest knife in the drawer but I get there eventually!)

I transferred a simple haas visual quick code (VQC) pocket milling file across onto memory stick and have attached bellow (hopefully!)

I tried your suggestions and re-named the file capital O and five digits per haas prog. Address (O00123) and used the Fanuc.cbpp. In post processor mac wrote $O=00123

I transfered the file (when in its script form i went save as and saved it to memory stick. Was that correct?).

When I opened it on the haas cnc toolroom mill  it seemed to be all there. All g-codes were visible on haas display. However each block was enclosed in brackets, and many of the dimensional values had “?” after them. See attatched picture.

I tried to run the prog. But (asI had expected)  it threw up an error “file beginning/ end marker missin” any ideas what to do?

Thanks

Mogtract

[10bulls]

Well I took a little stab at a Haas post processor.

It may still be a little way off, but I'd be interested to see if it offers any improvements.

One change I made, was to force the gcodes to have leading zeros (eg G01 as opposed to G1).
This may also be a problem with M codes as well, but unfortunately there are some M codes that
are hard coded in.  If you still get errors, try changing occurances of M3, M5 etc to M03 and M05.

I think the tool change, tool length offset commands need some more work, but if you can see if this at least loads and I'll put some more thought into doing those better.

I will be doing some work on the post processor for the next release with a view to adding more control over the gcode output.

[mogtract]

Hi 10bulls

I downloaded the zip file, unziped it and saved it in my documents.  I then followed your Post Processor System download "to make a post processor be used as a default fo all new drawings...." i then  created a new stepper motor mounting plate in cambam and generated gcode. When i went to view the "script" there were no "leading zeros" on the gcode, it  was the same as previously tried.

Am i doing something wrong ?
Is there another way to get it to recognise the new .cbpp ?

Thanks

Mogtract

[10bulls]

The .cbpp file needs to go in the following folder:

Program Files\CamBamPlus\post

CamCam will reload the post processor details the next time it starts.
If CamBam is already open, you will need to go Tools - Reload Post Processors.

Double check the correct post processor is selected under the machining properties of your drawing.
The default postprocessor in the drawing template will only be used for new drawings (or new documents
created opening a dxf or 3ds/stl file etc).

I am just going to check now that I attached the correct post file...otherwise I will feel like a complete spanner!

[mogtract]

That worked haas.cbpp in correct place.

Next problem !
I decided to create a simple pocket in order to figure things out one step at a time. I created code using your new haas10b.pp and loaded it into machine. Machine moved all axis and started spindle but then threw uo an error message "invalid I, J OR K in G02 or G03". On closer inspection there is a value of 0 beside all I`s and J`s.

I went back to cambam and tried producing g code with some of the other .cbpp which all gave values for  I`s and J`s. ? (no other value was changed just the post processor)

Any Ideas ?