M20 Threadmills

[jlw™]

So M20 has kinda always been my stop point for taps. What threadmills are you guys using for M20?

 

None of my goto's have an acceptable M20 sized threadmill. All I can find has a 10mm shank which is too small imo.

 

I want inserted threadmills for M20.

 

Thanks

[Machineguy]

I'm not a fan of inserted thread mills at that size. They pound to hard.

Harvey makes some multi tooth ones. Depends on depth. One pass.

[Guest]

Check out Carmex

 

http://212.235.101.236/Index.aspx

[jlw™]

Carmex is my preferred JP. I have a bunch of them. All C18 and C25 tho. I have tried a C12, it's a chatter maker and nothing more.

 

I could try some solids.

[Sticky]

I usually use solids for small sizes like M20 and under.

 

In regards to chatter, how many passes are you taking and are you appropriately adjusting your feedrate based on the tool diameter and bore size?

[g huns]

I have always used Harvey thread mills. Recently started using Walter-Titex. They cost a little more but seem to cut and hold up better.

 

Their 20mm is on a 16mm shank. They have long, short, coolant thru, no coolant through...

[jlw™]

g huns good sir, could you send me a link?

[jlw™]

I usually use solids for small sizes like M20 and under.

 

In regards to chatter, how many passes are you taking and are you appropriately adjusting your feedrate based on the tool diameter and bore size?

 

On the C18s I take 0.02in/pass with a 0.004in finish pass. On the C25s I take 0.03in/pass and a 0.006in finish pass. I always provide a spring pass but they usually get skipped. The C18 and C25 could take more and never chatter but I know exactly how many holes I can run the way I run them and I know how they size.  Those numbers are radially, not diametric.  I do not account for the diameter regarding feed, I program the feed for finish dia.

[g huns]

g huns good sir, could you send me a link?

 

How bout a screen shot?

 

610 are short, 611 are long. W1 is coolant thru, W0 is external coolant.

[Sticky]

On the C18s I take 0.02in/pass with a 0.004in finish pass. On the C25s I take 0.03in/pass and a 0.006in finish pass. I always provide a spring pass but they usually get skipped. The C18 and C25 could take more and never chatter but I know exactly how many holes I can run the way I run them and I know how they size.  Those numbers are radially, not diametric.  I do not account for the diameter regarding feed, I program the feed for finish dia.

 

If you want the best tool life and surface finish I would recommend correctly adjusting the feedrate. I'll make an example.

 

You have .5" diameter endmill, with 5 flutes, and you want to run 500sfm and a chipload of .001" per tooth.

 

You end up with S3820 and F19.1

 

If you want to take a .02" radial cut, and maintain your chip thickness, your feed needs to be increased to F48.7

 

Now, let's say you want to use all of the above data, but inside a .6" diameter bore.

 

Internal: Corrected feed = Nominal Feed * (Minor Dia - Cutter Dia) / Minor Dia.

 

Your feedrate is now F8.1

 

 

If you wanted to use the above cutting parameters but on a .6" diameter boss:

 

External: Corrected feed = Nominal Feed * (Minor Dia + Cutter Dia) / Minor Dia.

 

Your feedrate is now F89.3

 

 

I find when it comes to maximizing threadmill performance and life, these calculations are essential.

[gcode]

Check out Carmex

They have an outstanding online app for selecting and programming

threadmills

 

http://www.carmexusa.com/content.aspx?file=customerpages/software.htm

[jlw™]

If you want the best tool life and surface finish I would recommend correctly adjusting the feedrate. I'll make an example.

 

You have .5" diameter endmill, with 5 flutes, and you want to run 500sfm and a chipload of .001" per tooth.

 

You end up with S3820 and F19.1

 

If you want to take a .02" radial cut, and maintain your chip thickness, your feed needs to be increased to F48.7

 

Now, let's say you want to use all of the above data, but inside a .6" diameter bore.

 

Internal: Corrected feed = Nominal Feed * (Minor Dia - Cutter Dia) / Minor Dia.

 

Your feedrate is now F8.1

 

 

If you wanted to use the above cutting parameters but on a .6" diameter boss:

 

External: Corrected feed = Nominal Feed * (Minor Dia + Cutter Dia) / Minor Dia.

 

Your feedrate is now F89.3

 

 

I find when it comes to maximizing threadmill performance and life, these calculations are essential.

Thanks for the tip, I get the math. I have no clue how to do that in the threadmill unit, so I do as I have for over a decade and program it to the finish pass. I have always had excellent results.

 

I don't care how you adjust feed, a tool with a .629in cutting dia on a 10mm shank hung out almost 6 inches is gonna scream. That's why I'm tapping and looking for alternative threadmills. I got 16x m20 and 18x m24 another 4inches deeper all less than 1xD from the wall.

 

Now we're going from 4140ht to aeromet 100 and I have to find a threadmill.

 

Find me a threadmill then you can teach me how to run it!

 

For the record, I circle mill a lot of large round features and adjust feed accordingly.

[jlw™]

Thanks gcode, the C18 and C25 I run now are carmex and are my favorite.

[jeff]

My go-to for indexable thread mills is Vardex.

I don't think there is a thread out there that they don't have a tool for.

http://www.vargus.com/vardex/template/default.aspx?pCatId=30

[oneyankfan1]

Emuge and Walter both very good i use them on small holes alot. But recently we did a PIP with sandvik and they brought a NPT 1-11.5 threadmill that has absolutely killed everything so far, but it is $1009.00. I asked my rep if it had a comet dust substrate.

[gcode]

Emuge and Walter both very good i use them on small holes alot. But recently we did a PIP with sandvik and they brought a NPT 1-11.5 threadmill that has absolutely killed everything so far, but it is $1009.00. I asked my rep if it had a comet dust substrate.

try the Carmex Spiral Flute insert mill for 1" NPT

We do thousands of NPT holes a month and this tool blows away any anything we've tried

http://www.carmex.com/page.php?actions=show&id=193&instance_id=4

 

I don't know exact cost, but I'd guess $250 for the holder and $80 for the inserts

In a ridiged setup we routinely get a 100+ holes from a set of inserts in mild steels

cycle time is under a minute