carmex threadmill

[Tim Pruett]

I'm wanting to thread mill some 1/4 18  and 3/8 18 npt holes in p20 for coolant lines and baffles. Would a carmex thread mill # mt3312c06 18npt work ok? I'm worried it may not go deep enough. according to the info on their web site it only goes .58 deep. I have very little experience thread milling. tia

[gcode]

_{try this thread mill app}

_{It gives very good info}

_{This is their main website}

_{http://www.carmexusa.com/}

 

_{this is the link to download their thread mill app}

 

_{http://212.235.101.236/}

[gcode]

according to my Stellram thread mill app

a 1/4 NTP is .402 deep

and

a 3/8 NPT is .408 deep

I always run them deep though

 

a .58" LOC should be good for both sizes

[Tim Pruett]

Our 3/8 plugs and baffles have approximately .5" of thread. And we like for them to be under the surface when installed. So I wouldn't think that milling the thread to .41 deep would be deep enough. Am I missing something?

[Tim Pruett]

Carmex's thread mill app says to go 10.375mm deep which is .4085. I guess I will go ahead and get the tool and try it in a scrap piece of aluminum until I get exactly what I want.

Thanks for the help.

[Tim Pruett]

Oh man, just noticed I had 666 posts so I had to post this to get off of that number. lol

[The Cathedral]

Sounds to me like you're doing a sort of custom thread, in which case you'll probably not be able to use a standard tool. Unless you either a ) counterbore the thread to below the surface or b ) grind relief on the threadmill, once you get past the LOC on the mill you'll be rubbing the shank and wiping out your threads.

[Tim Pruett]

Ok , we have two different plugs. One of them is about .5 long and the other is .4. Our baffles are around .4 as well. So If I mill the threads around .425 deep this will let the plugs and baffles be installed just below the surface. Thanks for all the help.

[gabe525424]

Chamfer the top of the hole before thread milling you can pick up some extra depth.

[guitar]

_{try this thread mill app}

_{It gives very good info}

_{This is their main website}

_{http://www.carmexusa.com/}

 

_{this is the link to download their thread mill app}

 

_{http://212.235.101.236/}

 

 

That's a nice app

[gcode]

That's a nice app

yes it is

I recently used it for guidance doing 4-40 x .375" deep threads in titanium

The holes were up against the walls of a 2.5" deep pocket and required a 20" Capto

stack to reach the part.

Much to my surprise, it worked like a charm.

I'd been sweating those holes for months and the actual machining was so routine it was boring

[Tim Pruett]

Does anyone know if the carmex thread mill listed above has taper. When I use their app "taper" is not checked. I'm assuming it does even though it's not checked.

Also, is the speed and feed I get from their app for one pass, if so, could I feed a littler faster if I'm cutting the thread in 4 passes?

[gcode]

Carmex NPT thread mills are tapered

I use the bottom diameter to define the tool in Mastercam

I used to use a simple endmill definition for NPT thread mills

but the new thread mill tool in X9 works well so I am slowly changing my thread mill libraries over to the new thread mill tool definition

 

The Carmex app gives really good feedrates.

We normally calculate feed rates to the center of the tool

When you cut  the inside of an arc this can result in a chip load that is much too high

The Carmex app calculates the correct C/L feed rate then adjusts it so that the feed per tooth

is correct where the tool contacts the ID of the hole

If you want to calculate this yourself, the formula is

 

Ajusted Feed Rate =  Feed rate x ( (Hole Ø - Thread mill Ø)/Hole Ø))

[Tim Pruett]

Awesome, thanks for the info.

[mkd]

When gcode talks threadmill and carmex, you can take it to the bankB)