Make your first helix at the bottom of the hole, then come up 4 or 5 pitches in Z and mill another helix.
...And all the online thread mill program generators I've used online take the first helix at the bottom of the hole, however, when using thread mills with inserts having multiple teeth, I’ve had problems taking the first helix at the bottom of the hole if the length of the insert used on the 2nd pass is considerably less than the full insert length cut that would be used at the bottom. You could find the bottom of the hole cuts smaller than the top. Also, chatter is more likely when plunging in with the full length of the insert, especially if not arcing into the cut. Of course, this varies depending on material, tool setup, type of tool, etc and can be remedied by adding passes, editing speeds/feeds, etc.
I suggest you even out the cut length used on the insert by taking the first pass as close to halfway down the thread length as possible, then the second helix at the bottom of the hole. Depending on the length of thread, this may need to be done 3 or 4 times; whatever is necessary. The percentage of insert length that would work without problems will vary by application.
You could program something like so:
(.540 diameter cutter cutting 3/4”-14 thread X 1.125" deep):
G90
G54X0.0000Y0.0000B0.000
G43Z.1000H1
G1Z-.5627
G91
G1G41X.0525Y.0525D1F10.0M8
G3X-.0525Y.0525Z.0089I-.0525J0.0000F1.5
G3X0.0000Y0.0000Z.0714I0.0000J-.1050
G3X-.0525Y-.0525Z.0089I0.0000J-.0525
G1G40X.0525Y-.0525F10.0M9
G90
Z-1.1339F50.0
G91
G1G41X.0525Y.0525D1F10.0M8
G3X-.0525Y.0525Z.0089I-.0525J0.0000F1.5
G3X0.0000Y0.0000Z.0714I0.0000J-.1050
G3X-.0525Y-.0525Z.0089I0.0000J-.0525
G1G40X.0525Y-.0525F10.0M9
G90
G0Z.1000
Regards,
Paul