Pro-e Pro-man wildfire 2.0

[eglider]

I am having to learn pro-man on my own and after programming my first part which has to be rotated 17-degrees after machining the first set of features at 0-degrees the csys is off in the X-plane. Y and Z seem to be positioned correctly. The machine I am using is an older Mori Seiki SH-40 horizontal mill with rotary pallet. Is there something in the gpost I need to change or do I need to rotate the csys in the machine. I am not sure on how to rotate the csys in the machine. I need to know where to place the G68. The machine manual I have is not very clear on this move. Thanks for any help you can provide.

[rharter52]

add a csys for every face you want to machine on,then in the parameter page select sequence csys instead of machine csys.make sure your machine is defined as a 4 axis machine.

[JonasC]

Hej,

For every indexing position you want to machine 3 axis, but at an angle you will,as rharter52 said, need to add an extra coordinate system in ProE where your z axis is in the same direction as your tool axis.

Now, depending on how you want the actual output in the g code there are 2 options:

1)
Most common:
You want the machine to just rotate and still use your main coordinate system.
In this case you want to select the parameter in the sequence to Output_type = machine_csys. It doesnt matter (if you are using A,B,C) where the csys in ProE is located or even oriented. ProE will recalculate the local csys to the machine csys.
However if you are using PLANE SPATIAL or similar in a modern heidenhain you might need to think of how the coordinate system is oriented. (Could still be offsetted) This all depends on how the postprocessor is written.

2) If you want to use a local zero in your machine, you simply choose Output_type = sequence_csys in the sequence parameters. You might also need to put a numer in FIXTUE_OFFSET_NUMER parameter which would correspond to your local zero in the machine. I.e. 1 => G68 P1 etc. This also heavily depends on how your postprocessor is written.

I would simply start with alt 1 above and try if it works. If it doesnt or you really wanna go with G68 I would look into the postprocessor. There is some excellent training material on this on PTCs website. (maintenance required)
http://www.ptc.com/cs/cs_25/howto/ncgp4903/ncgp4903.htm

If you need additional help, dont hesitate to ask.

/J

[cncwhiz]

I might have a post you can use? I do programming for machines that are for the most part the same. I can give you a lot of pointers on this type of machining.