Issues with a milling post processor..

[Tm america]

I am having issues with a milling post processor . When doing a pocket it will do the inside part of the pocket but then when it should just move over and cut the outside part it will lift up then try to do the outer cut in mid air.. or say st safe z..This is really a problem when doing letters that are less than double the width of the bit.So you will end up having only the parts milled where it travel it traveled in the one direction.. i have tried everything i can think of and no change.. i am posting an example of the g code ..The first part is fine ..When it switches to the letters is where it messes up

[Les Newell]

Could you give me a copy of the job file (File->save job) with everything set up ready to cut. Also let me have a copy of the post processor.

[Tm america]

I will email them to you

[Tm america]

Les i just emailed them to you along with a description of what it is doing and which line is the first time it does it.Thanks in advance for your help

[Les Newell]

The problem is on line 372 in your post:
post.Text (" G01 F1270 z10")

post.Text simply outputs text to the gcode file. That means the post does not know the machine has moved. This is a better solution:
post.ModalText(" G01")
post.ModalNumber (" F", 1270, "0.0###")
post.ModalNumber (" Z", 10 * scale, "0.000")
post.Eol()

Now the post knows exactly what is happening so the generated code will be correct.

[Tm america]

Thanks i didn't even think of the possibility of it not knowing what it did due to Adding that part to the post..Makes perfect sense..Les you are always extremely helpful and knowledgable ..I will be testing it out with these changes and post the results.. Thanks again..

[Tm america]

Had to change the post.ModalText("G01") to post.Text("G01") otherwise it would post it the first time then it would not post it again for the z axis moves.. because the line would start with The f command it would ignore the z axis moves.. but it is working good now ..Thanks