Help please !!!!

DNGUYEN1 · 2009-10-15 13:43:52

Good morning to all,
This is a first time I build the machine Simulation for 5axis machine (vertical Mazak 815 FANUC CONTROL 15 IM) the machine simulation
looks good for 3 axis , but 5axis (machine simulation) it does not looks right , even I already tried for three different
controler in vericut the library and it still do same problem, I was wonderring is this the Vericut control issue? Do I need to modify
something inside the control ?
we programed by the tool tip and using G43.1the Pivot distand is 12.5918

Any have would be greatly appreciated.

D nguyen
Nex-tech Aerospace
Wichita, Kansas

DaveH · 2009-10-15 18:58:27

This is probably not a control issue, we have simulating G43.1 correctly for years.
It sounds like the machine kinematics may not be correct. Try testing the machine via
MDI, load the tool, turn on the offsets and MDI some simple movements. Do the rotaries
pivot about the correct location? Does the tool tip go where you expect it to? If the machine
does not move correctly via MDI I suggest you talk to somebody experienced in machine/control
configuration.

SergeV · 2009-10-15 19:59:02

Also you Kinematics should be built correctly.

The component tree for a Mazak Vortex 815 should look something like this:

Base
__Y
____Z (0,0,41)
_______B
__________A
____________Spindle (0,0,-12.5918)
_______________Tool
__X
____Attach
______Fixture
________Stock

DNGUYEN1 · 2009-10-16 15:18:43

Thanks for Respond, I tested the MDI which is rotate B30.deg
G0G90G54 X15.Y2.
G43.1H23Z3.825
machine look right on "Z" except X axis the tool tip pass to the point that I want it go to, roughly about 6.00 "OFF" in X

Here is my Mazak component tree look like

Base
---X
___Y
___Z (0 0 30)
___A
___B
___TOOL (-12.57463)
Do I need to switch From B and A axis in my component?

SergeV · 2009-10-16 15:24:58

The Vertex machines I have seen, were A attached to B, but go look at your machine to confirm the correct configuration. If the B is moving, does it rotate the A axis? or is it the opposite?

It will have a huge effect on the 5 axis moves.

DNGUYEN1 · 2010-02-05 14:43:59

I got machine working now, but I still have one issue with G49, everytime machine reach to
G49 in the program tools plunged into the part, so I have manually edit all my Z value to 15.00" high
before go home then work fine.

again thank you for your help

D nguyen

SergeV · 2010-02-05 20:22:14

On the real Mazak controller, by default, when the G49 is called, the tool offset is immediately canceled causing the machine spindle to move down. But many customers have changed this setting on their controls to avoid this dangerous behavior. In the VERICUT standard setting, we decided to go for the worst case. It is better to have a false collision than to miss a real one.

to change this in VERICUT:

Configuration > Word/Address...
Find G49

under the macro, TurnOnOffGageOffset, keep the Override value of 0, but remove the Overrride Text: IMMEDIATE.

-- the tool offset will only be canceled on the next Z motion.

DNGUYEN1 · 2010-02-06 15:29:41

It works like a charm, thank you Serge!!

D Nguyen

VERICUT Users' Forum

#1 2009-10-15 13:43:52

Help please !!!!

#2 2009-10-15 18:58:27

Re: Help please !!!!

#3 2009-10-15 19:59:02

Re: Help please !!!!

#4 2009-10-16 15:18:43

Re: Help please !!!!

#5 2009-10-16 15:24:58

Re: Help please !!!!

#6 2010-02-05 14:43:59

Re: Help please !!!!

#7 2010-02-05 20:22:14

Re: Help please !!!!

#8 2010-02-06 15:29:41

Re: Help please !!!!

Board footer