Need Help!- G41 in wrong block???

[bennyboy]

Hi all! I have a twin table woodrouter by rye with a bosch control.
All I want to do is cut a square aperture in a door using G41 to allow for various tool sizes etc but can't get it to work. PLEASE HELP!!!
Here is part of the program in question:

N10 G0 X-1700 Y-1016 Z0 START POINT
G91 incremental
G1 G41 Z-20 F1000 D2 D2 refers to diameter 2 in tool table
G1 Y-300 F5000
G1 X-300 F7000
G1 Y300 F5000
G1 X300 F7000
G1 Z0 F3000
G40
The position of G41 is apparently in the wrong position (ERROR; too many blocks suppressed!)
Can somebody please tell me where to stick it? (politely!)

[Kiwi]

G41 should be in a block with a X/Y movement, not Z movement.

[bennyboy]

Can anyone pinpoint exactly how to write in the g41?
think I've tried every thing but need some inspiration!!

[HuFlungDung]

For tool radius compensation to work, you need to initially position the tool off of the actual profile of the work. So to cut a square, beginning at a corner will require 6 movement commands while the tool is already at depth:
-first move from start point to a corner of the square as comp is turned on.
-4 commands to move around the sides of the square.
-1 move to take the tool off the profile as compensation is cancelled.

Think of a compensated path as one where the tool is switching from centerline on the path, to circumference tangent to the path. This requires a minimum lead in distance equal in length to the radius of the tool comp radius. While actually watching the machine, it may look like nothing has happened as comp is turned on if the minimum lead in distance was used, nonetheless, the control has recalculated its position with regard to the commanded endpoint adjusted for comp radius tangent.

So when machining a closed profile using machine compensation, you'll have to imagine adding lead in/lead out tails to the path yourself.

[beege]

Originally Posted by bennyboy Hi all! I have a twin table woodrouter by rye with a bosch control. All I want to do is cut a square aperture in a door using G41 to allow for various tool sizes etc but can't get it to work. PLEASE HELP!!! Here is part of the program in question: N10 G0 X-1700 Y-1016 Z0 (START POINT) G91 (incremental) G1 Z-20 F1000 G1 G41 Y-300 D2 F5000 (D2 refers to diameter 2 in tool table) G1 X-300 F7000 G1 Y300 F5000 G1 X300 F7000 G1 Z0 F3000 G40 The position of G41 is apparently in the wrong position (ERROR; too many blocks suppressed!) Can somebody please tell me where to stick it? (politely!)

G41 placed as above in red should get your comp turned on correctly. The G41 is going to shift the tool path to the left of the programmed geometry, whether cutting a pocket or an outside contour

G40 should also be used with an X and/or Y move, such as:
G40 Y-300

[Kiwi]

Originally Posted by beege G41 placed as above in red should get your comp turned on correctly.

If N10 G0 X-1700 Y-1016 Z0 is the START POINT of the square, the comp should be turned on before this point.