[SolidCAM_13]

As the title says. I need to know if a Multus can perform helical moves when using G137. Has anyone done it and are there any special requirements?

[OkumaWiz]

Last I heard Helical milling is an option for Y-axis. Definitely one worth having...

We use it all the time on our machines, but we've always had to order it as an option.

Best regards,

[budgieW]

You will get a better result using XC. G137 works best for 2 axis moves

[cncDecoder]

G137 allows programming of XY coordinates, but automatically translates them to XC coordinates.
As far as I can see, G137 as a coordinate conversion function only allows 3-axis moves X Y & Z with linear moves using G101.
G102 & G103 are XY moves only.
The best option will be in G138 mode, and the X Y & Z axis with G2/G3 commands.

[cncDecoder]

For reference of those that may search for the answer to this post in the future,
helical moves in XC are an optional extra offered by Okuma (as most features that are "standard on other machine makes" :tired.
Make sure to ask for this option known as Profile Helical Cutting.
In addition, ensure to ask for DNC-DT, VSST, Super Nurbs, Thread Phase Matching, Thru spindle air, Tool Centre Point control - yes these are optional.

[Algirdas]

Thread Phase Matching option is only convenient way to thread phase match. Every Okuma lathe with C axis offset does the same by means of proper setting of C axis offset

[cncDecoder]

Thread Phase Matching is for use with thread turning - so no C-axis settings are going to make a difference.:tired:
The function allows you to easily chase an existing thread, by effectively getting the machine to record the position as you manually move your tool to inline with the thread root.
Handy option for jobbing work.

See the attached instructions for Thread Phase Matching on a Multus.

[Algirdas]

no C-axis settings are going to make a difference
not exactly. I agree, the option is usefull. It's possible to do the same playing with C axis offset (and Z axis offset, of course). You need to do a little work and understand how it works. Z axis synchronization with C axis do the thread mach and nothing else. Correct me if I am wrong

[fordav11]

with normal turning threading the C axis is not used so offsetting it wont do anything. the normal way is to offset Z but it gets very difficult when re-working tapered threads and internal threads. if you have info on using the C offset to re-work threads I'd like to hear more....

[Algirdas]

the c-axis encoder is used for spindle and Z axis synchronization. There is nothing more, but Okuma's control accuracy magic.
I'll try to explain briefly. Let's say, we have a workpiece with thread and we need to cut the same thread again. Add to your tool X offset enough it would be out of material for settings. Make a part program with thread cycle. Start the program. Switch to single step mode inside threading cycle. watch animation and go step by step until you have a moment just before Z axis threading feederate. Here is your exact Z position of thread start.
Now we will set c-axis offset for this thread.
select "mid-auto manual", stop the spindle. Take your tool moving Z axis to location, where thread is already on it's nominal dimension. (Normally this program stop inside threading cycle must be outside material in Z axis direction). Take tool tip to thread edge (see note 1) moving X axis and C-axis (note 2).
Go to zero offsets and calculate. Guess your C axis value. Z axis offset must be calculated the moved by mid-auto manual distance.
Proceed with manual spindle start, "return from mid-auto manual" and tool proper X offset.
That's short explanation. Try, and you will discover all missing details.
note 1: You can use the zig-zag threading infeed in program, then you must do an extra check - repeat the same procedure on next thread cycle step.
note 2: you can leave C-axis untouched. Z movement is enough.

[Algirdas]

the c-axis encoder is used for spindle and Z axis synchronization (Z-axis encoder involved, sure), since there is no separate encoder. There is nothing more, but Okuma's control accuracy magic.
I'll try to explain briefly. Let's say, we have a workpiece with thread and we need to cut the same thread again. Add to your tool X offset enough it would be out of material for settings. Make a part program with thread cycle. Start the program. Switch to single step mode inside threading cycle. watch animation and go step by step until you have a moment just before Z axis threading feederate. Here is your exact Z position of thread start.
Now we will set c-axis offset for this thread.
select "mid-auto manual", stop the spindle. Take your tool moving Z axis to location, where the thread is deep enough. (Normally this program stop inside threading cycle must be outside material in Z axis direction). Take tool tip to thread edge (see note 1) moving X axis and C-axis (note 2).
Go to zero offsets, guess your C axis value and calculate. Z axis offset must be calculated on the basis of moved distance by mid-auto manual.
Proceed with manual spindle start, "return from mid-auto manual" and restore proper tool X offset.
That's short explanation. Try, and you will discover all missing details.
note 1: You can use the zig-zag threading infeed in program, then you must do an extra check - repeat the same procedure on next thread cycle step.
note 2: you can leave C-axis untouched. Z movement is enough.