Welcome, Guest. Please login or register.
Did you miss your activation email?
September 02, 2014, 01:51:04 PM

Login with username, password and session length
Search:     Advanced search
* Home Help Search Calendar Links Login Register
+  Machsupport Forum
|-+  G-Code, CAD, and CAM
| |-+  G-Code, CAD, and CAM discussions
| | |-+  G42 problem
Pages: « 1 2 3   Go Down
Print
Author Topic: G42 problem  (Read 6448 times)
0 Members and 1 Guest are viewing this topic.
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #20 on: December 03, 2006, 03:43:08 PM »

Email me your DXF file and the code generated by Lcam and let me see what we are talking about.

You can get my email by clicking on my user name above the picture of my car.

Graham.
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #21 on: December 03, 2006, 04:27:11 PM »

Graham....The Lcam file and the tap file are on its way to you..You are more than welcome to post it here and show the file here..please do..I forgot the dxf file I will resend...Michael
Logged
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #22 on: December 03, 2006, 05:49:45 PM »

Michael,

No DXF file yet.

Graham.
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #23 on: December 03, 2006, 06:37:06 PM »

I resent it to you zipped up
Logged
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #24 on: December 04, 2006, 03:50:12 AM »

Hi Michael,

I have looked at your files and all look OK,  I think the problem is with Lcam, its just not putting the compensation size (P) or a tool offset (D) into the code.

This is what I would do :-

Create your programs with Lcam

Set a tool length and diameter in the tool offset table, use tool 1 with a length of 0.00 and a diameter of .0625"

On the first G41/G42 in your program add D1, you do not need to do this for every G41/G42 as D1 is global.

e.g.

N5 (File Rib1 )
N10 (Default Mill Post)
N15 (File Posted in Mill Mode)
N20 (Sunday, December 03, 2006)
N25 G90 G80 G40 G91.1
N30 G0  Z1.0000
N35  X1.3309  Y1.9273
N40  Z0.2500
N45 M3
N50 G1  Z-0.1250  F10.00
N55 G42 D1
N60  X1.5034   F15.00
...........

This will make Mach use the tool offset you set in tool 1 for the compensation on the contours.

Try this with the tool just scratching the face of the material, you should be able to measure the size to comfirm all is well.

This is what my Sim gives as the profile.

Graham.


* Rib1.jpg (24.74 KB, 600x348 - viewed 215 times.)
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #25 on: December 04, 2006, 09:46:54 AM »

Thank you Graham...I didn't know you could do that with the tool offset feature..I would like to be able to make a whole table of wing ribs on one tap file and having to scroll down the multi thousand line list would not be fun, putting in P.0625 at each G 42...Thanks again for your effort!..Ill let you know how it turns out..Michael
Logged
ger21
Global Moderator
*
Offline Offline

Posts: 3,892



View Profile WWW
« Reply #26 on: December 04, 2006, 10:32:28 AM »

If you can get a copy of AutoCAD 2002, I have a macro that will output the g-code directly including the G42's, including the Px.********* You'll need to draw the leadin and leadout moves yourself, though. Let me know if you need a link to it.
Logged

Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #27 on: December 04, 2006, 11:16:10 AM »

In my opinion the 'P' version of G41/42 is dangerous and a pain to use.

If you have any more than one in the code there is always the chance one could get missed when editing the size, also the code has to be output to an editor and reloaded just to do this.

Not only that but why should you have to change a whole load of them when changing 1 offset value will do it all.

It is far better to use 'D' with compensation, not only do you have the diameter offset but also the wear offset to compensate for minor tool variations.

There is the bonus of being able to have the contour in a sub program and using it for both roughing and finishing just by changing the 'D' number in the main program. If anybody wants to see how this is done, ask

Learn to do it like the professionals do it,  FORGET THE 'P'

Graham.
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #28 on: December 04, 2006, 08:41:53 PM »

Well...I had my first successful cut today...that rib...I went down the list and inserted the P.0625all the way down..12 times...because each hole was cut twice at two different depths,and then the outside profile twice...next is to try the D1 way..Can"t thank you guys enough..I am having fun again

To ger21..I do have ACAD 2000...it was' E'asy looking for it by the BAY if you know what I mean... Wink...because people upgrade all the time  but they hardly ever let go of things above 2002..If you let me know where I can find 2002 it would be much appreciated...Thank you also for the help...It was really getting frustrating there...Michael
Logged
Pages: « 1 2 3   Go Up
Print
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines Valid XHTML 1.0! Valid CSS!