Please help me with this Strange thread

[behnod]

Hi everyone.
we are asked to machine a part with a strange thread .
the part is 180 mm in diameter that should be variably threaded ( G34 in fanuc ) with a 25 mm circle insert . ( the profile of thread is 25 mm semicircle )
the problem is that because of the machining load on 25mm insert i'm gonna use a 8mm insert instead .
i can use software to create the 25mm semicircle profile with 8mm insert but i don't know how to make it variable because this strategy is not available in cam softwares .

the picture shows the compensation of 8mm insert for 25mm profile .


Regards
behnod

 

[angelw]

Hi everyone.
we are asked to machine a part with a strange thread .
the part is 180 mm in diameter that should be variably threaded ( G34 in fanuc ) with a 25 mm circle insert . ( the profile of thread is 25 mm semicircle )
the problem is that because of the machining load on 25mm insert i'm gonna use a 8mm insert instead .
i can use software to create the 25mm semicircle profile with 8mm insert but i don't know how to make it variable because this strategy is not available in cam softwares .

the picture shows the compensation of 8mm insert for 25mm profile .
View attachment 162006

Regards
behnod

Hello behnod,
What you need to do is treat the Thread as a Multi Start Thread, but instead of indexing the the Starts equidistant (angle wise) around the circumference, the multiple starts will be indexed to the extent whereby they generate a Single Start fashioned by the 8mm insert. You can make use of the data obtained from your software to establish each new Z start point to index the new thread lead and the depth for that thread start. If you can imagine your drawing placed so that the Left most tool position is clear of the start end of the workpiece, then all of the intersecting vertical and horizontal lines indicate the the Z Start and Depth for that particular Start.

Personally, I would write a Macro Program to calculate the Z index points and Thread Depth, passing detail such as the Radius of the Thread Form, Initial Pitch etc. The Tool Rad being used could also be passed as an argument, or read from a Tool Offset Registry by the Macro Program.

Regards,

Bill

 

[behnod]

Hello behnod,
What you need to do is treat the Thread as a Multi Start Thread, but instead of indexing the the Starts equidistant (angle wise) around the circumference, the multiple starts will be indexed to the extent whereby they generate a Single Start fashioned by the 8mm insert. You can make use of the data obtained from your software to establish each new Z start point to index the new thread lead and the depth for that thread start. If you can imagine your drawing placed so that the Left most tool position is clear of the start end of the workpiece, then all of the intersecting vertical and horizontal lines indicate the the Z Start and Depth for that particular Start.

Personally, I would write a Macro Program to calculate the Z index points and Thread Depth, passing detail such as the Radius of the Thread Form, Initial Pitch etc. The Tool Rad being used could also be passed as an argument, or read from a Tool Offset Registry by the Macro Program.

Regards,

Bill

Thanks Bill .
I am so thankful for the time you took to help with my question.
actually what i think to do is to gather the start points of each pass from the software and put every path in a G34 format but as you know it is a very time consuming way .(the more it be smoother the more the line would be )
personally i would prefer to do whole in the software but it seems that there is no software available to do that .
by the way i don't have any information about macro programming .

 

[angelw]

Thanks Bill .
I am so thankful for the time you took to help with my question.
actually what i think to do is to gather the start points of each pass from the software and put every path in a G34 format but as you know it is a very time consuming way .(the more it be smoother the more the line would be )
personally i would prefer to do whole in the software but it seems that there is no software available to do that .
by the way i don't have any information about macro programming .

Hello behnod,
Either you can alter the Post Processor to output the code including the G34 blocks, or another way would be to write a Macro program that contains the bare bones code to execute the G34 Block to the finish point on the Thread and return to start. This Macro would be called using G66 instead of G65 (you will need to read up on the use of G66 - its in the Fanuc Manual and not very difficult). Then following the G66 Call Block you would have all the coordinates obtained from your Cam Software for the Z Start and X values. The Macro Program will be repeated as each of the coordinate blocks that follow the G66 Block are executed. At the conclusion of the coordinate blocks, G67 is specified to cancel G66 Mode.

Regards,

Bill

 

[behnod]

Hello behnod,
Either you can alter the Post Processor to output the code including the G34 blocks, or another way would be to write a Macro program that contains the bare bones code to execute the G34 Block to the finish point on the Thread and return to start. This Macro would be called using G66 instead of G65 (you will need to read up on the use of G66 - its in the Fanuc Manual and not very difficult). Then following the G66 Call Block you would have all the coordinates obtained from your Cam Software for the Z Start and X values. The Macro Program will be repeated as each of the coordinate blocks that follow the G66 Block are executed. At the conclusion of the coordinate blocks, G67 is specified to cancel G66 Mode.

Regards,

Bill

dear Bill .
that's the solution . i'm gonna edit the post processor .
Thanks so much .

Regards,
Behnod