[Ridings]

I have a .742 dia single point thread mill cutting a 7/8 - 9 thread. When I type 0 in for the Clearance Dia it wants to start at G0 G90 X0. Y.065, which I need to start at 0 because the dia hole is only .7638. In addition, it makes the Z depth go the distance that I want
Z.1
G91
G1Z-.595F18.
But when I type in a clearance dia of like .700 it wants to start at X0,Y0 but it makes my new Z move go lower. Gibbs want to change my new Z move to
Z.1
G91
G1Z-.6344F18.

Please any advice would help

Thanks

[montie]

Your clearance diameter will need to be larger than your tool diameter and smaller than the hole size. Also post this question or do a search at GibbsCAM Support Forums - Powered by vBulletin. You will most likely find more information there on this subject.

[Ryan Jagoda]

Can you post your file?

[Ridings]

Hello Ryan
Here the one I have going to a Clearance Dia of .750 trying what montie suggested
N3
T3M6
G90G0X0.Y0.S1200M3
G43Z1.H3M8
Z.1
G91
G1Z-.6208F18.
G0X.0018Y.0018
G41G1X.0027Y.0002D3
G3X-.0045Y.063Z.0258I-.0045J.0314
Z.1111J-.065
Z.1111J-.065
Z.1111J-.065
Z.1111J-.065
Z.1112J-.065
X-.0514Y-.1048Z.0394J-.065
X.0526Y.035Z.0258I.025J.0194
G40G1X-.0015Y.0023
G0X.0003Y.0025
G90Z.1
G90G0X-.0593Y0.
G91
G1Z-.6208
G0X.0018Y.0018
G41G1X.0027Y.0002D3
G3X-.0045Y.063Z.0258I-.0045J.0314
Z.1111J-.065
Z.1111J-.065
Z.1111J-.065
Z.1111J-.065
Z.1112J-.065
X-.0514Y-.1048Z.0394J-.065
X.0526Y.035Z.0258I.025J.0194
G40G1X-.0015Y.0023
G0X.0003Y.0025
G90Z.1
M9
G91G28Z0.M19
G28Y0.
G90
T1M6
M30
%

The Problem is I have a Z of -.495 and Z to finish at .100. I fully understand that its in incremental and it will add .100 to my Z. My question is why is my Z -.6208 not Z-.595

[Ryan Jagoda]

I meant for you to post your Gibbs file, the one you are using to generate this code. However, looking at your generated code, it seems that it is making a partial radius move onto your cut. The distance traveled in Z is .0258, or the difference between -.6208 and -.595. Slightly under 1/4 of a full rotation on a 9-pitch.

If you turn on balloons and hover over the "clearance diameter" dialog box, it mentions that it will move to a specified point, make a helical approach into the cut, then thread mill. Same thing moving off.