Need Help!- Thread Milling on v22

[PinMan]

I am wondering if anyone has used this feature and how'd it work out for you? I am starting a new project and am considering using a thread mill instead of a tap.
I need to put a 1-8 thread 1.5" deep in 6061 Aluminum. As I have hundreds of parts to do, I think that thread milling will be a better option than tapping.
I am currently waiting on some tooling to come in and thought I would get your guys' opinions on how well BobCAD's thread milling works.

Thanks for any help and advice.

[moldmker]

Just looked at the Thread feature....I haven't used it but was was impressed with the options available.

However, I did a quick program for 1"-8 threads with Arc Move Output selected. No Z moves were output for the helical revolutions, only the leadin and leadout (Fanuc6M post). These are easy enough to add to the code, but begs the question of whether the rest of this feature was tested at all.

The Line Move Output code looked OK, but I used this type of code from v21 and it makes the threads look faceted.

Ended up writing simple incremental sub programs and calling them at hole locations.

Good luck,
moldmker

[PinMan]

I have done the same, using both the arc moves and the line moves. I ran into the same problem with the Z moves (Fagor8055 post). Actually transfered it to my mill and run the mini program, sans tooling, and control alarmed for improper code. Still trying to figure that out.

Did the same thing with the line moves and it seemed to run ok, but without a cutter to test it out, I am concerned about the end result having a faceted finish. As you stated.

I dont have any previous experience with thread milling, so for tooling, I ordered both a solid cutter and an indexible one to test out. Which one seems to work better?

[moldmker]

Looked inside my post and added the z_f to line 64:

64. Arc move.
n, g_arc_move,x_f,y_f,arc_center,z_f,feed_rate

Now it outputs the Z coord on the helical moves. (Didn't test it yet for negative effects)

I never used the insert style mill, only the carbide 60deg woodruff looking type.
That's so I can accommodate custom pitches for mold shrinkage.

Looks like best bet for your depth and quantity would be a full form cutter? They make for a lot less passes, unless time is not a factor.

Also just noticed that the v22 thread milling feature doesn't have tapered pipe option.

moldmker

[HMB3000]

Originally Posted by moldmker (Didn't test it yet for negative effects) moldmker

I think the testing on "Negative effects" from using the software has been done. Not sure if the final report is finished yet.

[PinMan]

Thanks for the post edit. It added the Z moves perfectly

A question comes to mind, as I haven't done this before. Are thread mills designed to take it all one pass or should you take multiple passes? If multiple passes are needed, do you just make more toolpaths on BabCAD until you reach the thread size?

[HMB3000]

Originally Posted by PinMan Are thread mills designed to take it all one pass or should you take multiple passes? If multiple passes are needed, do you just make more toolpaths on BabCAD until you reach the thread size?

I use thread mills in cast steel and cast iron. We run a 11 TPI- 4 hob flute.1 1/2 oal flute lenght. The hole depth is 1.4. we have a program written to do it in 2 steps in Z at one cutter comp. vaule and then back out go back in run the same code with a new CCV. This is should done for pipe thread as they have a taper. The reasl draw back of thread mills is one chipped tooth and not you have to do it in more than one pass. we do it in two passes as this is a large casting and it is safer to let the thing run twice. Than have to re-work one part

[PinMan]

Cool, thanks for all the info. Hopefully my tooling will be in today and we will see how it goes. I am going to try both to see which is better and I will let you guys know the results

[Textralia]

Originally Posted by PinMan I am wondering if anyone has used this feature and how'd it work out for you? I am starting a new project and am considering using a thread mill instead of a tap. I need to put a 1-8 thread 1.5" deep in 6061 Aluminum. As I have hundreds of parts to do, I think that thread milling will be a better option than tapping. I am currently waiting on some tooling to come in and thought I would get your guys' opinions on how well BobCAD's thread milling works. Thanks for any help and advice.

I'll save you some time.....


It Does't work!

I'm hoping to sell my Bob Scam.... It's a joke!

[PinMan]

Thank you so very much for your insight. If you aren't going to back up your claim with useful information, I would appreciate it if you would keep your trash talking to threads of the appropriate venue.

And just to let you guys know, I had tons of success with it. Only needed very minor changes to the post and the thread came out beautifully.

Again, thank you guys for your help and productive comments.

side note: Textralia, check your facts before you post things to keep yourself from sounding like an idiot.