[RoboElvis]

Hi all.

We machine aluminum bodies on a Mori Seiki MH-40 for air regulator applications. Inlet - 7/8-14-UNF3A Outlet - .825-14 NGO-RH-EXT. Around .80" thread length.

It takes us what seems to be forever (30+ seconds per port) to cut the inlet and outlet ports. We currently use a 6 point threadmill insert.

Here is the question i have... Would going to a full length (if they make them) insert allow me to make one revolution make sense? I know that I may have to take a few, smaller, cuts to reduce tool deflection. What about a single point tool? Seems there might be something to making one good pass all of the way out.

They've tried chaser heads and have had bad burring issues. Obviously, because of the application, we can't have that.

Any ideas or experiences would be appreciated on this one.

Thanks in advance,

[cdlenterprises]

Theoretically speaking, yes a longer insert will allow you to decrease the # of revs, less deflection, form issues, etc. That sounds like a long time to thread mill. What are your speeds/feeds?

[RoboElvis]

I'll post in our thread milling macro. I haven't gotten to deciphering that part of the code yet. There are two passes because the insert length is shorter than the threads being cut. They're also doing a spring pass to clean up from any tool deflection.

*snip*
S6000F30.T53
G0G90G43H68D68Z12.2M8M3
S8000F100.
G66P4007D[#512+.02]Z#513W.0714C5.T.78
...
...
O4007(THREAD MILLING MACRO)
#110=#5001
#111=#5002
IF[#3NE#0]GOTO100
G0G91X-.39
G0G91G41X0Y[#7/2+.0304]
G90Z[#26+[#23*2.027778]]
G91G3X.39Y-.0304Z-[#23*.027778]R2.
G2J-[#7/2]Z-#23
G2J-[#7/2]Z-#23
G3X.39Y.0304Z-[#23*.027778]R2.
GOTO200
N100
#100=[#3*#23]
#101=FUP[#20/#100]
N150
#101=[#101-1]
G0G90G40X#110Y#111
G91Y.3473
G91G41X[#7/2-.0304]Y0
G90Z[#26+#100*#101+#23*1.027778]
G91G2X.0304Y-.3473Z-[#23*.027778]R2.
I-[#7/2]Z-#23
X-.0304Y-.3473Z-[#23*.027778]R2.
G0Z1.25
IF[#101NE0]GOTO150
N200
G0Z1.25
G40G90
M99
*snip*

It looks unnecessarily cumbersome. I tried to install the threadmilling wizard i found a link toon the forums here. Stupid administrative rights. The IT guy is in another plant so i can't install it.

My goal is to make the code as simple as possible. Our operators also do setups and I want to help them understand what the machine is doing.

[HuFlungDung]

I would imagine that you could get a boost by using a solid carbide threadmill. It will give you enough length to do the thread in one pass, and four times as many cutting flutes, so you should be able to mill as fast as you would dare with one.

[cdlenterprises]

Here is some sample code for threadmilling that I use on one of our jobs. It's for a 5/8-36 thread. Thread mill was .5 dia single lead.


:T18 M6
G0 G90 X1.75 Y12.906 C0. S7000 M3
Z.1 M8
G1 Z-.75 F65.
G91
G1X.068F5.
G3X0Y0Z.86087I-.068J0.K.02777
G1X-.068
G90
G0Z2.
X1.75 Y1.75
M00


All you need to do is program a G3 with a K in addition to the I & J. The Z move is simply your thread lead. X0 Y0 on this part was actually the lower left corner of the part but if you switch to G91 over the hole (thereby making the center of the hole X0 Y0) the code becomes pretty simple.

Just be sure to change back to G90

This doesn't do anything for your cycle time issue but it may help you make operators understand what's happening.

:cheers:

[big_mak]

Take Hu's suggestion. Solid Carbide Thread Mills Can Kick som serious a$$ especially in aluminum. You sould be able to really give'er.

Check out Vardex webpage. Don't be affraid to push it.

[ajl6549]

Hi all.

We machine aluminum bodies on a Mori Seiki MH-40 for air regulator applications. Inlet - 7/8-14-UNF3A Outlet - .825-14 NGO-RH-EXT. Around .80" thread length.

It takes us what seems to be forever (30+ seconds per port) to cut the inlet and outlet ports. We currently use a 6 point threadmill insert.

Here is the question i have... Would going to a full length (if they make them) insert allow me to make one revolution make sense? I know that I may have to take a few, smaller, cuts to reduce tool deflection. What about a single point tool? Seems there might be something to making one good pass all of the way out.

They've tried chaser heads and have had bad burring issues. Obviously, because of the application, we can't have that.

Any ideas or experiences would be appreciated on this one.

Thanks in advance,

Absoleutly! Check out Iscar cutting tools. We use them all the time and they work great. We cut iron, steel and alu. and brass etc. Deeper thread depths would require more passes but most of the thread mills are long enough to cut 2x dia. The tool I'm refering to is like a solid carbide end mill but it has the thread pitch on it. You just position at the hole bottom, heli-arc into the work helix up one thread, and heli-arc out. Be aware they are a bit pricey but very well worth it.