VERICUT Users' Forum

JimV

Member

From: Santa Fe Springs, CA

Registered: 2006-08-02

Posts: 25

Website

Tool with two Z offsets.

Help!
I have an old program that uses a keycutting endmill. This keycutter has two Z offsets (H7 & H17).
The bottom of the keycutter uses H7 to control the lower surface of an undercut and H17 controls the upper surface.  (The difference between H7 and H17 is the actual tool flute length)
How do I get Vericut to recognize the second H17 offset?  :?
Thanks!

---

v6.2.1
Auto-Diff, OptiPath
No Machine Simulation
__________________________________________
Dell XPS 410, Intel Core2 @ 2.13GHz
4GB memory, NVIDIA GeForce 8600 GT video card
Vista Home Premium

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: Tool with two Z offsets.

make sure you use a Library control as they are configured for multiple offsets. otherwise look at the Word/Address for any Fanuc in the Library for the macros called for H, it should call GageOffsetDrivenPoint.

In Tool Manager, select your tool, right-click Add Driven Point, rename the first one 7 (default is 1).
right-click Adriven Point again, rename to 17. highlight 0 0 0 under the Description column, with the middle mouse button, pick the top of the key cutter (middle-mouse button will only register the Z value).

Also make sure Project > Processing Options > G-Code > Settings
Programming Method = Tool Length Compensation

JimV

Member

From: Santa Fe Springs, CA

Registered: 2006-08-02

Posts: 25

Website

Re: Tool with two Z offsets.

Thanks Serge!
It worked great...I would of never figured that one out.
I did notice in the Log file there was an "Error: Driven Point offset: 1, was not found".
So I added a Driven Point 1 back in with 7 and 17 just to see what would happen and ran it through without an error. Is this correct?
Anyway, thanks again for your help.

---

v6.2.1
Auto-Diff, OptiPath
No Machine Simulation
__________________________________________
Dell XPS 410, Intel Core2 @ 2.13GHz
4GB memory, NVIDIA GeForce 8600 GT video card
Vista Home Premium

SergeV

Senior Member

From: Irvine, CA

Registered: 2004-10-08

Posts: 507

Website

Re: Tool with two Z offsets.

Glad it worked!

the Driven point 1 might be necessary if you have H1 called. But if there is no matching driven point found, it gives an error but still gets the gage length from the tool definition.

If there is a matching driven point, the gage length will be the distance between the driven point and the gage point.

p-cnc

Member

From: Toronto, ON

Registered: 2004-11-11

Posts: 36

Re: Tool with two Z offsets.

Serge,

Today I got same problem, I searhed I found this. I set-up what ever you showed in this post. But some reason it doesn't work for me. Did I do something wrong or missed something?

Thank in advand.

T86, H16 and H18

Here is NC file:

N815 G0 G90 X.6494 Y-.3
N820 G43 H16 Z3. M8
N825 M3
N830 Z.1
N835 G1 Z-.2
N840 G41 D19 X.7494
N845 G3 X1.0494 Y0. I0. J.3
N850 X-1.0494 I-1.0494 J0.
N855 X1.0494 I1.0494 J0.
N860 X.7494 Y.3 I-.3 J0.
N865 G1 G40 X.6494
N870 G0 Z3.
(GROOVE TOP, USE H18 LENGTH OFFSET SET)
(MILL 2.65+.10MM GROOVETOP,H18 TO TOP OF TOOL)
N950 G0 G90 X.6494 Y-.3
N955 G43 H18 Z3. M8
N960 M3
N965 Z.1
N970 G1 Z-.1
N975 G41 D19 X.7494
N980 G3 X1.0494 Y0. I0. J.3
N985 X-1.0494 I-1.0494 J0.
N990 X1.0494 I1.0494 J0.
N995 X.7494 Y.3 I-.3 J0.
N1000 G1 G40 X.6494
N1005 G0 Z3.
N1010 M9
N1015 G91 G28 Z0. M19
N1020 G49

p-cnc

Member

From: Toronto, ON

Registered: 2004-11-11

Posts: 36

Re: Tool with two Z offsets.

Bump !!!!
:cry:

p-cnc

Member

From: Toronto, ON

Registered: 2004-11-11

Posts: 36

Re: Tool with two Z offsets.

Never mind. I used newer control, it work fine.

Thanks