mpmaster_horizontal

[zebra]

Im trying to use postprocessor for horizontal machine center with mastercam x5. When im posting my operations i have this error:

Error- select machine achievable toolplane with y-axis along machine y - set and repost

Whats wrong?

[K2csq7]

When im posting my operations i have this error:

What kind of operations do you have?

Have you successfully used this Post,MD,CD combination before?

That error usually comes out because you have a rotary operation and your Machine Def is not set up correctly

[Chris McIntosh]

The calculations for the rotary axis in the post are based on the setup in mastercam. Are you programming as a horizontal or a vertical machine (ie is the top toolplane B0 or is the front toolplane B0)?

 

For horizontal machines, the default setting is to program using the front toolplane as B0, the right plane as B90, back as B180 and the left as B270 (depending on the direction of rotation). Make sure you have oriented your part correctly for horizontal machining.

 

The error you are getting is because the toolplane you are using in an operation has it's Y-axis not oriented in the correct direction.

 

If you are programming as a horizontal machine, the toolplanes Y-axis must align with the world Z-axis (the Z-axis of the WCS plane). In this case you can get the correct toolplane by rotating the front toolplane about it's Y-axis.

 

If you are programming as a vertical, then the Y-axis needs to always align with the world Y-axis (the Y-axis of the WCS plane). To get the correct toolplane orientation, you can create your planes by rotating the top toolplane about it's Y-axis.

 

Bottom line, make sure the Y-axis is oriented in the same direction for all tool planes you are using.

[Joe788]

^What Chris said.

 

You need to have WCS set to top, and then use Front for B0, right for B90, back for B180, left for B270 (and for anything in between, stick with that same type of orientation, with Y axis of your TPlane going parallel to the Z axis of the TOP WCS.)

[zebra]

The calculations for the rotary axis in the post are based on the setup in mastercam. Are you programming as a horizontal or a vertical machine (ie is the top toolplane B0 or is the front toolplane B0)?

 

For horizontal machines, the default setting is to program using the front toolplane as B0, the right plane as B90, back as B180 and the left as B270 (depending on the direction of rotation). Make sure you have oriented your part correctly for horizontal machining.

 

The error you are getting is because the toolplane you are using in an operation has it's Y-axis not oriented in the correct direction.

 

If you are programming as a horizontal machine, the toolplanes Y-axis must align with the world Z-axis (the Z-axis of the WCS plane). In this case you can get the correct toolplane by rotating the front toolplane about it's Y-axis.

 

If you are programming as a vertical, then the Y-axis needs to always align with the world Y-axis (the Y-axis of the WCS plane). To get the correct toolplane orientation, you can create your planes by rotating the top toolplane about it's Y-axis.

 

Bottom line, make sure the Y-axis is oriented in the same direction for all tool planes you are using.

 

 

Im using free post and machine definition :Mpmaster - Master G-Code Post - Version X5

I attached example.

21085.MCX-5

[Chris McIntosh]

So the issue here is that your wcs is set to the same plane as your toolplane/construction plane. Set your wcs to top in both operations and then post out the code and you should be good to go. If you are using a different work offset (G54/55/etc) for each plane, you can just change the work offset value on the planes screen.

[dforsythe]

The calculations for the rotary axis in the post are based on the setup in mastercam. Are you programming as a horizontal or a vertical machine (ie is the top toolplane B0 or is the front toolplane B0)?

 

For horizontal machines, the default setting is to program using the front toolplane as B0, the right plane as B90, back as B180 and the left as B270 (depending on the direction of rotation). Make sure you have oriented your part correctly for horizontal machining.

 

The error you are getting is because the toolplane you are using in an operation has it's Y-axis not oriented in the correct direction.

 

If you are programming as a horizontal machine, the toolplanes Y-axis must align with the world Z-axis (the Z-axis of the WCS plane). In this case you can get the correct toolplane by rotating the front toolplane about it's Y-axis.

 

If you are programming as a vertical, then the Y-axis needs to always align with the world Y-axis (the Y-axis of the WCS plane). To get the correct toolplane orientation, you can create your planes by rotating the top toolplane about it's Y-axis.

 

Bottom line, make sure the Y-axis is oriented in the same direction for all tool planes you are using.

 

When using the mpmaster hz post you will get this error any time your try 5 axis drill and are not in “mastercam top with front, left, right or back or userer defined” We do a lot of front and back work then the part needs to go onto a mushroom riser for side holes. To get this orientated properly we have to rotate the top plane 90 deg ccw about the x direction. Next you rotate that plane 90 deg about the x axis. This gives you a user defined top and front with Y going up as it should. I’m not sure when it started X4 or x5 but it will freezes all your tool paths and give you an error saying some or all operations In this file will not run on this machine. The work around for now is to make a copy of the model which is poor practice so we do not use mastercam for hz programming anymore. I really need to dig deeper and find out root cause so we can use it again. If anyone has any ideas please let me know.

 

[Guest ZEBRA]

HOW CALL NEXT TOOL AFTER COMMAND TOOL LENGTH COMPENSATION (G43)?

NOT LIKE THIS: T1 M6

[K2csq7]

You should have this in the post...

 

stagetool   : 0 	#0 = Do not pre-stage tools, 1 = Stage tools

[Chris McIntosh]

In the control definition you need to select the tools menu and then select the "enable staged tool routines" check box.

 

Then in the post you need to make sure that the next_tool$ variable is on the same line as your tool length compensation:

 

     pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$