post processer for mach 3 3+2

[stephen.brindle]

hi I am trying to get my 3 axis milling machine to 3+2 

but I want to rotate the b and c axis by hand (no motors) I have looked at a 5 axis post that works but it compensates for the tool and gives wrong cutter position 

so what I am asking for is a post 3+2 for manual change of b and c axis ,so after that I can re datum the cutter and it will mill

or how to change this 5 axis post so there is no compensation of tool on b and c axis 

I am using mach3 mill 

thanks steve

[engineguy]

@stephen.brindle 

Stephen, are you wanting the mill to do an operation, stop and you just do a manual index or are you going to be manually turning the non motorised axis continually ???

[DarthBane55]

Create a setup for each orientation that you need, so the operations do not have a tool orientation in them, and it will not output any angle change.  Just add M0 when it changes setup.  It will output the code in relation to each setup's origin.

[stephen.brindle]

hi I am wanting the mill to do an operation, stop and I just do a manual index  maybe b or c axis 45 or90 degree on ether axis then reset the tool to a datum and it does the next operation I am using fusion 360 and it lets you orient the tool  in different directions( like I said before I have a 5 axis post but it compensates for the tool length and rotation )

any help would be great thanks steve

tried to upload picture but it wont let me 

[DarthBane55]

That's what I was explaining.  Maybe not clearly though...

Create 1 setup for each orientation you need.  

Put M0 between the setups, in order to do your manually index.

Then it will go to the next setup, with correct work offset as you set in that setup.

[stephen.brindle]

hi don't really understand

say I am milling a car for example

on my 3 axis machine I can cut the bonnet  (hood) and roof  

if I wont to cut the front bumper I would have to turn my cutter 90 degrees (b axis)

if I wonted to cut the side I would have to cut it the other way 90 degrees (c axis )

and the back 180 degrees  (b axis) I think I need a 3+2 post for mach 3 that work in fusion 360 or a 5 axis that can be adapted 

I am doing manual rotation and resetting the tool every rotation,  and in fusion I am only doing a program for each cutter path (not all in one ) hope this makes sense thanks steve

[DarthBane55]

Hi, because you will be doing the indexing manually, you don't need a 3+2 post.  The 3+2 post would output the code for an automatic indexer, which you said you don't have.  So if I take your example:

-make a setup from the top, to machine the hood and roof.

-make another setup tilted for the front bumper, etc etc

When you code this, it will not output any index moves, because you will be leaving the operations without a tool orientation.  Since the tool orientation is done inside the setup itself, the post will not even know that you are tilting.  It will output all coordinates in relation to the WCS defined in each setup.

That way, once the hood and roof are done, you have a M0 in your program with a comment telling your to manually index to required angle for the front bumper.  Once you've done the indexing, you continue the program, and it will machine the bumper correctly, as long as you define the WCS in your setup correctly.

If you don't understand, let me know, I'll make a simple sample of this, it will then become clear.

[engineguy]

@stephen.brindle 

Stephen, what is really needed is the actual configuration of your machine, if you have a Trunnion type indexer (A and C axes configuration) that is on the bed of your machine then what @DarthBane55  is trying to do for you will work, create a toolpath turn the indexer to the required angle, touch off your tool and cut the toolpath. As has been suggested for that scenario all you need is the basic 3 axis Mach3 Post Processor.

However if one of your Axes is on the Head (Swivel head A and B Axes configuration) then that is going to be a bit more involved so please upload a photo of your machine, that will make it much easier for @DarthBane55  to do an example program for you. If it is a swivelling head that rotates then it a whole different way of working.

So please let the Community know what is the configuration of your machine, to upload a photo click on the Camera Icon at the top of your Post and that will open a path to your computer that says "Choose Files", just navigate to where you have saved the photo and select the one you want to upload and click "Open" and the image file "preferably a .jpg format" will be uploaded and inserted into your Post.

[DarthBane55]

@engineguy oh that makes sense, I had assumed that OP had a mechanical indexer, thus doing the indexing manually, but I could be wrong, and it could be that for a reason or another he will index the machine in jog mode.  Thanks for asking for the clarification.

(side note: you'll be happy to know that now we can drag and drop pictures in the posts, it works great! (that is fairly new)).

[stephen.brindle]

Hi I think I get it but can you do a sample I don’t get the m0 the other thing I don’t get is if I do this in fusion with a mach 3 post it won’t post out the bumper one but if I use the 5 axis post it works but it adds the tool length and spin compensation so no good for me unless I can change post thanks for your advise

[stephen.brindle]

 

[engineguy]

@stephen.brindle 

The M0 command is a simple "Machine Stop" command which would be inserted after each operation so that you can do your indexing.

Please, you still haven`t answered the question regarding the configuration of your machine, just a photo or a link to the make and model of the machine, this is critical to getting any sort  of sample program, the poor guy is trying to help you and you are just going over and over irrelevant stuff that is holding him back 😞 😞

Regards

Rob

[stephen.brindle]

 tut 90 on both photos thanks

[engineguy]

OK, now we see the photo, went up while I was typing, thanks very much, something to work with for you @DarthBane55  now 🙂 🙂

[DarthBane55]

Attached file.  You'll have to adapt it to your setup, but you'll get the idea.  

-1 setup per orientation.

-M0 to tell you to index manually.

-different WCS number for each setup, so that you can set all faces needed with its own WCS in the machine.

I think it should help...  hopefully!  😮

EDIT: I just realized, if you cannot post the file with your post, change the tool number...  it's possible your post doesnt support so many tools (our machines support 999 tools, but most standalone machines only have 30 to 40).

[stephen.brindle]

 hi sorry these are the only photos I have the machine is s post and arm retrofit single and motors 

[stephen.brindle]

Hi so I put that file as my post processed or is it a example in fusion ? Thanks again steve

[DarthBane55]

Upload the file to Fusion, you'll then be able to open it and see what's going on.

[stephen.brindle]

Hi yes put that int fusion some more photos of set up
The thing I don’t get is if the a axis travels down the side of the car then on your example top x is correct going to side the x is going up
So does the soft wear no the axis’s have changed
So example x becomes y So y travels down the side of the car hope this makes sense

[boopathi.sivakumar]

Hi @stephen.brindle

If my understanding is correct , you are expecting fusion to output the codes based on single origin (Setup origin),

even the tool is orientated on a specific angle you are expecting the output values from the setup origin.

But currently the fusion outputs respect to the local workplane.

If you want to output with respect to single origin then you can edit the post processor to do so

  var tcp = false;                 // Change this to true
  if (tcp) {
    setRotation(W); // TCP mode
  } else {

 go and edit the post and search for var tcp

and change it to true instead of false.

now post will output with respect setup origin

test it carefully and let me know the feedback