Newbie- Tapping on a CNC

[behindpropeller]

A few tapping questions.

1. Is it a good idea to always center drill holes that will be used for tapping?

2. Are there any special holders needed for rigid tapping? My assumption right now is to just put the tap in a collet of the correct size and go with it. If not..please post a link to a correct tap holder.

3. I'm assuming 0-1/4" holes need a tap and thread milling should be used on larger holes? It seems like the lower torque of a TM series mill lends itself to thread milling with a higher spindle speed.

4. Since I do 99% prototype work I am thinking I will want a single point thread mill. Does anybody have a suggestion for a single point thread mill??


Thanks

Tim

[tobyaxis]

Originally Posted by behindpropeller A few tapping questions. 1. Is it a good idea to always center drill holes that will be used for tapping? 2. Are there any special holders needed for rigid tapping? My assumption right now is to just put the tap in a collet of the correct size and go with it. If not..please post a link to a correct tap holder. 3. I'm assuming 0-1/4" holes need a tap and thread milling should be used on larger holes? It seems like the lower torque of a TM series mill lends itself to thread milling with a higher spindle speed. 4. Since I do 99% prototype work I am thinking I will want a single point thread mill. Does anybody have a suggestion for a single point thread mill?? Thanks Tim

#1, yes, it provides a Lead for the Tap

#2 a floating holder is a good idea

#3 Tapping up to a 1/2-13 should be fine and if you want Peck Tap and make sure you flood with a good coolant.

#4 single point thread mills are good but Insert Thread Mills are better.

Cheers

[tobyaxis]

BTW: when buying taps get the Spiral Helix. They draw the chips out instead of standard gun taps the push the chips down.

Also Multiple Insert Thread Mills are even Better and you can feed faster.

[Geof]

I routinely spot drill going deep enough to leave a small chamfer when the tap drill does the hole.

Taps smaller than 3/8" I hold in ER16 collets, larger in ER32 and of course I have Rigid Tapping turned on.

The largest taps I have used successfully in a MiniMill which is similar in power to a TM are 1/2"-13 and 9/16"-20. I have stalled the spindle with larger ones and with pipes taps larger than 1/4" NPT.

I always use 1000 rpm no matter whether it is aluminum, leaded steel, C1018 cold rolled or hot rolled or C1045. On all sizes I use peck tapping unless it is a through hole only about 1 diameter deep; on C1018 and C1045 I am very conservative and may only peck two revolutions a time.

Someone else can suggest the thread mill; I think Iscar has some but they are available from many sources.

[Matt@RFR]

Originally Posted by behindpropeller A few tapping questions. 1. Is it a good idea to always center drill holes that will be used for tapping? 2. Are there any special holders needed for rigid tapping? My assumption right now is to just put the tap in a collet of the correct size and go with it. If not..please post a link to a correct tap holder. 3. I'm assuming 0-1/4" holes need a tap and thread milling should be used on larger holes? It seems like the lower torque of a TM series mill lends itself to thread milling with a higher spindle speed. 4. Since I do 99% prototype work I am thinking I will want a single point thread mill. Does anybody have a suggestion for a single point thread mill?? Thanks Tim

1. Yes, because the more accurately located your drilled hole is, the less likely the tap is to have to go off center and probably break. But don't use center drills, use spotting drills. You can feed them like hell and they are MUCH less likely to break. Plus, with a spotting drill the correct size, you can chamfer the hole and spot the hole in one go, saving quite a bit of time. http://www.lakeshorecarbide.com/spotdrills.aspx

2. I've held taps from 2-56 to 5/8-18 in collets. No problems whatsoever.

4. All depends on quantity of parts and the specific threads you're cutting. I have a few single point thread mills that I used for prototype jobs with odd ball threads. For example, 3.125-38 and 1/4-50 threads. Good luck finding off the shelf inserts for those! Scientific Cutting Tools is a good source.

[DSL PWR]

1-3 is already well covered. #4--> I like micro 100 single point tools for smaller holes (less than .75"). I have an insert type threadmill, but you need about .75" to do an internal thread. One other draw back to the inserted tool is you only have one cutting edge, so it takes a while to make a thread. With the micro 100 you get 3+ cutting edges so your feed rate is much better. http://www.micro100.com/

[tobyaxis]

Thanks DSL PWR you reminded me of the Mini Thread Milling Hobs. They are a bit pricey though but for a single pass tool they are tops in Aluminum.

[behindpropeller]

Thanks for all of the replies.

Tim