What's new
What's new

Catia V5 and MAKINO EU64 Tilt Wire

trickchit

Plastic
Joined
Feb 23, 2016
Anyone out there using a Makino EU64? I'm using Catia V5 R24 to program a slot in the end of a pin to enable a 1/4 turn retention method. I get the correct motion for what is actually two separate cuts, one at a plus 15 degree angle and the second at -15 degrees but my motion is not centered on the pin where it should be. My program origin and geometry are at the center of the .250 inch diameter pin which sits 2.100 inches above the table. My G95 line reads G95P2.1Q2.225Z#5015. I'm using a CIMPRO post where my lower guide offset is the distance below the program plane and my upper guide is set at the distance above the program plane. The post is using the distance from the lower guide for output.
 
trickchit,

Are you processing this geometry as a T - Taper program or as a 4-Axis program? From the sounds of it, I believe you might be overcomplicating the process and defeating the machine.

You should not be programming or inputting the machine Guide Heights in your CAD/CAM system. The machine control knows where the Upper and Lower Guides are in relation to the work table, and the control will automatically compensate for the true fulcrum point of the wire against the guides. From the programming perspective, you should be creating your programs from actual part geometry as if the part were sitting on the Zero Line table. If you are processing this as a 4-Axis program, you will also need to include a "P" value on the same line as your Cutter Comp G41/G42 command, and this tells the machine how to compensate and digest the U/V position moves. The correct "P" value is determined however you program and have your CAM Post setup, but the "P1" value is by far the most common.

P0 = No machine control compensation...whatever U/V value you have in the program is where the machine will position to
P1 = Machine control will compensate for the Guide Heights, and the U/V moves have been calculated as INC moves from the X/Y
P2 = Machine control will compensate for the Guide Heights, and the U/V moves have been calculated as ABS moves from the X/Y

You can also contact Makino's Technical Support at 1-888-625-4664 to discuss this in greater detail with the Applications Group.


-Brian
 
Hi Brian,
Thanks for the reply. I am driving the part as if it was a five axis part though using only four. Due to the part geometry I initially enter the part at a 15 degree angle and cut the slot that is open to the end of the pin. I re-enter through this slot, make a thirty degree axis change, never breaking the wire, and and machine the remaining slot that is perpendicular to the first slot and rotated thirty degrees on the centerline of the pin. I have it cutting correctly now. I misunderstood the lower guide offset required by my post processor and had entered the table to lower guide distance when it actually wanted my Z0 (programming Z origin) to lower guide offset. Had I not found your earlier posts where you brought to light the G95 line requirements I would have never been able to resolve my problem. My cutter (wire) is defined as an .008 inch diameter tool with no P0, P1, or P2, D offsets, or cutter comp. It is driven as if it was a milling cutter climb cutting.

I have never tried to drive this used machine in tilt wire mode before and time permitting will take your advice and try to make it work the way you have explained. When you say Zero Line table do you mean the actual machine table? The operator had the center of this pin perched in a "V" block 2.100 inches above the table which is where I created my NC origin or WCS and 2D part geometry on an XY plane at.
 
trickchit,

The Zero Line Table refers to the actual work table top surface. This surface is the origin point that is used to establish the Guide Heights within the machine, so all Taper and 4-Axis machining will reference this point using the G95 command to understand where the work piece and geometry are located in the Z-Axis.

Take a look at the attached image, as the Taper Data (G95 Command) will look like one of these (4) examples when machining Tapers and 4-Axis programs. In all the (4) examples, the P-Program Plane value would change if the work piece was raised above the Zero Line Table, but the Q-Sub Plane value would remain the same. Below is basic information on the G95 command.

G95 P_____ Q_____ Z#5015
- G95 = Taper Data Plane Command
- P = Program Plane (Start location of angle from Zero Line Table Height of the program geometry)
- Q = Sub-Plane (Machining height/thickness of angle. Use ± values to control direction. Always the Incremental height value from the Program Plane)
- Z#5015 = Automatically reads the current set position of the G53 Z-Axis and establishes the Upper Guide Height location for program execution.

When processing Taper programs, the Q-Value (Sub-Plane) can be a (+) or (-) value. A (+) value places the taper above the programmed geometry (Example 1 & 4), whereas a (-) value places the taper below the Programmed geometry (Example 2 & 3).

When processing 4-Axis programs, which requires (2) different geometry profiles, the Q-Value (Sub-Plane) should always be a (+) value, and must be the EXACT distance between the (2) geometry profiles used to create the NC program.

-Brian
Taper Data Info.jpg
 
Brian,

I attempted to send you a personal message relating to this topic. Please let me know if you receive it. The message is not showing in my sent folder.

Thanks.

-Mitch R.
 








 
Back
Top