I have experience for same case:,
Just insert M0 before angle changes.
And - you must "emulate" functions like TRAORI, M128, G43.4, and CYCLE800, PLANE or CYCLE19, G68.2
Thank you for reply!
This seems to be similar router machine. In our case the machine is FlexiCAM with E-CNC controller.
Can you explain me how can I set up tool in the machine? I need to know offset from the tool tip to the spindle for that? Or I will set up vertical tool and all other calculations will be done in the postprocessor?
Maybe you can provide me an NX file and G-code example?
1. Three Dx Dy Dz from tool mount to 4-axis rotary axis
2. Tool lenght or - if your CNC allow use vars - use tool lenght as var
Next - very easy - you need to recalc CNC position depend rotary angles. Thats all.
dont remember suppress circular output in case where your rotary axes are on the head, even at least one of them
I saved once one discusion simillar to yours I think.
I want taht somebody can comment this and put down his opinion
*** start of email thread ***
A customer who is machine tool builder has building a 5-axis Head Table engraving machine.
He has developed his own controller which does not have RTCP functions. (No Traori, G43.4)
Can we support such a machine using our post builder.
For a table-table machine I know this is possible, not sure about Head-Table configuration.
This is what we used to do all the time before the TCP was an option. Tool lengths must be precise and you must input the pivot distance into the post if you are not using simulation. The post will calculate the correct X Y Z output based on the pivot distance, tool length and MCS location. Everything will be in G43 mode. If you define a machine tool and have that in NX the kinematics from the machine tool will be loaded into NX at the time of post processing and will get the necessary information of the pivot distance, tool length all relative to your MCS location
Must enter opposite from 4th to 5th axis offset.
Can somebody describe these dimensions on simple picture?
What about location of zero point – and programing in nx/location of MCS ?
MCS must be 弹劾 center of the table
** end of email thread ***
What opinion are you waiting?
All items of your discussion don't take into account that: 1) tool length is a variable value when worker prepares tool assembly; 2) workpiece may have random position on the table.
That's why it isn't possible to calculate all exact coordinates during postprocessing. In addition you should write some subprograms for NC unit to re-calculate XYZ using: a) postprocessor output data; b) variables (see above); c) pivots.
Just now I have finished postprocessor for 5-axis head-head CNC for MACH3. Let me know if you dont see video, I use YouTube link.
1. You can use ANY tool length. I recalc tcp point INSIDE NC-Programm, no need to re-generate toolpath for new tool lengt.
2. You can use any G54 G55 G56 etc.
3. For this CNC-Machine for head I have some excenric beetween rotary axis, NX post compensate it.
I want to know if stuff in discussion above was right - parameters setting in PB off pivots etc.
In such machines worker should prepare tool lenght like in simulation and workpiece position. it is a rule I think.
I am interested what way to recalculate XYZ according to tool length in NC program use @Chigishev