Tapping Delrin 5

[rwild]

Looking for suggestions on tapping Delrin. I will need to tap a 1/4-20 through hole. The Delrin is 1.5 inches thick. I would prefer to do it in a CNC mill if that is possible. Information on the type of tap, coolant, or no coolant, cutting feeds, and speeds etc.

 

[TVP]

Here are some basics:

http://www.plasticsintl.com/documents/Guidelines for Machining Engineering Plastics.pdf

Section 12

http://plastics.dupont.com/plastics/pdflit/americas/general/H76838.pdf

 

[rwild]

Very helpfull links, Thanks TVP

 

[mfgenggear]

rwild

the only advice I can add is the tools for plastic need to have a knife like edges for the cutting tools, & as nicely posted by TVP speeds are high as possible. coolant is advisable to prevent melting of the plastic. recommend contacting a rep for coolant type.

I worked for screw machine shop where turning & milling
delrin was done often. the tools where normally made by the operators. unless it was milling & tapping on the mill.

 

[TVP]

My personal experience is similar to mfgenggear with respect to tool edges-- they need to be as sharp as possible, otherwise they just kind of gouge and rip the plastic. Regarding coolant, it is not necessary as long as you are in the sweet spot of feed and speed, meaning high feed rates so that there is no dwelling of the tool. Drilling of Delrin is pretty easy, it is facing and edge cuts that are more difficult with regards to local heating and surface effects.

 

[btrueblood]

I can agree with high feed and speed for Delrin, except when tapping. Machine tapping plastics has always given me grief, I generally avoid it - if the material heats up due to friction with the tap, it will "seize". It's probably due to the form of the cutting edge on the taps, and would be improved by having a tap specially made for plastics, but I never have the time and $ to go look for those. When necessary, machine starting, and then finishing the tapping by hand is my preferred method.

 

[MikeHalloran]

If the hole is not blind, and the fixture doesn't block chip exit, maybe a spiral point/ spiral flute tap could push the chips forward and out, but that's a very deep hole to tap by any means.





Mike Halloran
Pembroke Pines, FL, USA

 

[sbriar1]

Is this a blind hole or thru hole ?

if it is a thru hole just use a pully tap with collant and use a feed of 10 IPM and X that by your threads per inch.
We tap a lot of delrin without any problems by just using standard machining practices.
If this is a blind hole you will need to peck tap about .3 away from the bottom and finish by hand tapping, I would peck tap at about .25 per peck just to clear the chips and also have your rapid at about .4 above the part so the chips will get washed away by the collant.

 

[ABritTurner]

I've never used this material, it seems like a plastic. depending on how many holes you have to tap you should source the right tap for the material. I am in the Uk and always used the best taps available and discarded old taps, old taps can cost you a fortune when/if breaking on an expensive workpiece.

There are a number of considerations when tapping depending on the amount of work you have to do.
1. Find a supplier who can supply you specially made taps for all application don't just but from standard suppliers, go out of your way to find a dealer who has a direct contact with a manufacturer.
2. In the UK a grade of tap know as 1066 was the best tap for difficult materials, it was a specially coated tap
3. Arrange with your customer the maximum core diameter, you should be able to remove 25% above the minimum core diameter to ease tapping operations
4. Unless you are an absolute expert use a tapping head with a set clutch for tapping, if you are an expert then use the CNC
5. If the material is similar to nylon it will bind if the workpiece heats up, use plenty of coolant and tap by hand or tapping head.
6. If you have volume work to do then source a tap with clearances and back rake for the material you are using.
7. Ask your tap manufacturer for the correct speeds and cutting compound for the material you are working on.

When I ran my own business I spent from £10 - £100 for specialist taps on each job and always came out a winner by using a tapping head. We very rarely broke a tap and discarded old taps. Tapping difficult jobs needs to be planned with the proper taps, cutting compound and correct speeds.