Thread Milling

[jdholbrook33]

I've been doing a lot of tapped holes lately and wanted to use a thread mill instead of a regular tap (Gun tap is what I use now).

I picked up a thread mill from Maritool. 

https://www.maritool.com/Cutting-Tools-Thread-Mills-Metric-Thread-Forms/c78_135_137/p861/Thread-Mill...  or see the attachment.

Basically drop in the hole, move to the axial cutting depth, spiral up or down one revolution, move to center of hole, pull out.

Has any one done that with Fusion?

Care to share your method?

Thanks

James

[LibertyMachine]

All the time. Use the Threadmill operation under the 2D tab, not the one in the drilling dialog. There is no support for form tools, so you will have to just make an endmill of the appropriate diameter of cut.

If you've drawn the minor diameter, you will need to offset the cut, there is a section for that.

I'd suggest 1-1/2 turns if using a full form.

As always, run the tool above the part first, make sure your clearances are set right. Tools can last long if treated right, very short if you go bump

[Anonymous]

@LibertyMachine, do you set the number of turns with heights, top height= bottom height+1.5 pitch?

David

[LibertyMachine]

Personally, this is how I do it. First off, always make sure your clearances are solid. Nothing worse than blowing up a  $100 tool because it didn't come out of the hole before going full rapid to the next one. (I know you've been using Fusion for a while, so that comment was for anyone else that might be new and finds this thread)

Lets say I'm doing a 1/4-20 UNC tap

Top Height: Bottom of hole. The cool thing about many fields in Fusion, it takes math inputs. So, in the add'tl offset, type: 1/20*1.5. Unless this has broken in the most recent update, this will give you a positive offset of .075"

Bottom height: Bottom of Hole

I will set it to Multiple Passes. 2X with a .002-.003" offset

And do make sure "Drill tip through bottom" isn't selected. Threamills don't endcut very well 🙂

When you drill the hole, if you are using faces to drive the toolpaths, you will be fine. If you are manually entering in depths because you are using points, make sure your drill depth is proper to allow clearance of the tool  (.005-.01" is all that is needed)

Beware though, it will rapid into your hole. I've no issue with this, as that is also how Esprit ($20k CAM) puts out the code. I've not tried making it adhere to a plunge feedrate, as I'm accustomed to it

[Anonymous]

Yeah, I've also gotten used to the rapids, normally I use the Seco thread milling wizard or SmiProg (Swedish tool dealer Smicut) for thread milling calculations. Right now I'm doing M30x3.5 threads in steel, 48mm deep. Tool length is 49.5 mm, real scary stuff... The insert is 21mm high, how would you deal with multiple depth thread milling?

And by the way, @LibertyMachine, do you ever find time to sleep?

David

[LibertyMachine]

Sleep? What is this sleep you speak of.... 

For multipul depths. hmm. Through hole? That's going to require some thought and math. I've not done it in Fusion, but in Esprit I would go "top down" in 3 Z depths. Drop in on center, 16mm first depth, helical lead-in, 1.5 revolutions up. At that size threadmill, I'd probably add another pass, maybe 2 passes at .01" offset and one finish pass of .004". Next pass you would have to drop down another 16mm and repeat. And one more time for the final depth. You will need to verify in the code that the Z position after arcing in is 16mm more than the previous section. That's the only way to ensure you have the threads lined up right. Are you gaging the hole, or making it to fit a mating piece?

[Anonymous]

It's a through hole. This is the code I get from SmiProg:

S2016 M3

G00 G91 Z-52.

#1=3

#2=0

WHILE[#2LT#1]DO1

G01 G41 X1.778 Y-1.778 F88

G03 X1.778 Y1.778 Z0.438 I0. J1.778

G03 X0. Y0. Z3.5 I-3.556 J0.

G03 X-1.778 Y1.778 Z0.438 I-1.778 J0.

G01 G40 X-1.778 Y-1.778

G00 Z-4.376

G01 G41 X2.06 Y-2.06 F98

G03 X2.06 Y2.06 Z0.438 I0. J2.06

G03 X0. Y0. Z3.5 I-4.12 J0.

G03 X-2.06 Y2.06 Z0.438 I-2.06 J0.

G01 G40 X-2.06 Y-2.06

G00 Z-4.376

G01 G41 X2.25 Y-2.25 F105

G03 X2.25 Y2.25 Z0.438 I0. J2.25

G03 X0. Y0. Z3.5 I-4.5 J0.

G03 X-2.25 Y2.25 Z0.438 I-2.25 J0.

G01 G40 X-2.25 Y-2.25

G00 Z16.625

#2=#2+1

END1

G00 Z-11.

As you can see, it runs bottom-up, three radial cuts/depth. I would prefer to go top-down, just like you suggest, but Smiprog doesn't give me that option. Now I just wanna get this finished, but next time I think I'm gonna try doing it in Fusion.

Metric threads this size (M20- M30) are insane, btw, too big pitch at too small dia, anyone who's tried to hand-twist any of those know what I mean.

David

[LibertyMachine]

Here is something that I "think" should work just fine.

My advice about reading the code was incorrect, simply becuase I am not ending up where the previous section was starting. I failed to take into account eh length of the Full-Form. My advice would have been accurate if I was using a single profile tool.

EDIT: Removed .f3d file to correct brain-fart. I don't want people using this thinking it's right.

EDIT#2: Updated .f3d file is attached. 

The trick with multi-depth threadmilling is that not only do you need to take the depth of the hole into account, you also need to calculate out your thread pitch, Z depth of initial cut, 1.5 revolutions, depth of subsequent cuts, etc. Fun times...

[Anonymous]

That looks just great! But, correct me if I'm wrong, shouldn't the partial depth be divisible (hmm...is that the english term?) with the pitch? In this case , 14 (3.5x4) or 17.5 (x5).

[LibertyMachine]

Are you going off my most recent upload? My first attempt was a result of doing too many things at once and not putting full thought into it.

If you look at the v3 upload; First depth is 17.5, second is 35. The pitch is evenly divisble amongst them, 5 revs. I'm left with the balance of the part and I want to make sure the threadmill goes below the bottom surface, but not too far, given the length of the tool. So, I opted for 4 revs, or a 49mm depth.

The first depth is entirely arbitrary, more or less. Where it matters is the subsequent depths lining up to the initial. Of course, bearing in mind the final depth as well as length of tool

[Anonymous]

Yep, I looked at v1. 

And divisible WAS the word!