User Specified Home Return

mcam · 2013-09-29 20:46:48

On our Okuma MU500, we have specified a G30 P5 command.

This performs the following movements in order:

Retracts on Z to upper limit
Moves to X negative limit, and Y positive limit

In the control file, I have specified G30 P5 as follows:

Zaxismotion (Value 900)
Processmotion
Xaxismotion (Value -900)
Yaxismotion (Value 900)
Processmotion

I set no movement for the two rotary axes, as I want them to remain in their current position.

However, when I run the command, The Z axis, X axis and Y axis all move at the same time, and both the C and A axis return to their zero positions. How do I change this to move on Z first, then X and Y, and with no rotary motion? (which is how the machine moves)

Regards,

Mike

Verifun · 2013-09-30 01:44:05

It's strange how VERICUT behaves sometime...

I'm sure there's something we're doing wrong, as I'm experiencing a similar issue as you can see on my previous post about Z axis...

What you did is what I would do as well...

I noticed there's a combination which is G30 and P5...

Any chance G30 alone is defined in the control and is taking precedence?

Verifun · 2013-09-30 02:25:45

Well,

I made some changes in the Okuma VMC from the sample library and got what you wanted... it does not have rotaries but the order of events in XYZ occured as you expect... I guess it would work with a 5 axis Okuma as well...

Notice I used ?AxisMachineRefMotion instead of ?axismotion like you mentioned since you want the movements to occur relative to the reference point right... but then instead of entering +/-900 as the values, you could enter 0 as the value in the ?AxisMachineRefMotion macros and set the reference location in the machine location tables in the last pic... then there you could set that the reference point is +/-900 from the machine origin... just a different way to achieve the same...

In case you may want to change the machine reference location:

Verifun · 2013-09-30 02:35:10

Could not resist...

I loaded the control I changed in the previous post in the 5 axis Hermle machine from the library and run a G30 P5 command...

It worked as expected and the rotaries did not move...

mcam · 2013-09-30 07:53:42

Hi Daniel. Thanks for the comprehensive reply. I've not long got home, so I will look at this first thing tomorrow.

G30 is not defined by itself, so it wasn't misbehaving

VERICUT Users' Forum

#1 2013-09-29 20:46:48

User Specified Home Return

#2 2013-09-30 01:44:05

Re: User Specified Home Return

#3 2013-09-30 02:25:45

Re: User Specified Home Return

#4 2013-09-30 02:35:10

Re: User Specified Home Return

#5 2013-09-30 07:53:42

Re: User Specified Home Return

Board footer