NPT 3/4-14 internal thread

[wojtek90]

Hi

I have to do NPT 3/4-14 internal thread in 4140  0.75 thick plate.

There some pockets on the top of plate and coupler will be screw on the other side of plate.  Can I do it in one operation ( the taper will be wider on the bottom then on the top) using  ISCAR indexable  threading endmill with NPT 14 insert (11 tooth) ?  Should I use  minus value for taper , going from top to bottom?

Any suggestion on feed and speed  how many passes?

Any help appreciate.

[AHarrison1]

You will have to do this thread from the other side, unless you happen to have a reverse taper thread mill that is.

 

in mastercam you can add a taper to the operation.

 

Edited June 23, 2021 by AHarrison1
added picture

[gcode]

It is going to be difficult doing this from the back side of the thread

You will have to draw a tapered helix which will yield a point to point tool path

and the single point thread mill cycle time will be very poor

Even worse, you won't be able to gage the thread

I would use a full length Carmex tapered thread mill.

Cycle time will be about 20 seconds a hole

The Carmex Thread mill wizard is your friend

[wojtek90]

On 6/23/2021 at 5:47 AM, AHarrison1 said:

You will have to do this thread from the other side, unless you happen to have a reverse taper thread mill that is.

 

in mastercam you can add a taper to the operation.

 

Thank  you. I will ask ISCAR  about putting  insert in opposite direction.

[AHarrison1]

SO you are still considering cutting these in 1st op?

As mentioned by Gcode and myself, this will not be an easy feat.

You will not be able to gauge the thread. There will be more work needed to be done to cut the reverse taper. etc, etc, etc.

Some also recommend running a tapered endmill or reamer to give you the minor diameter taper and reduce the stress

on the upper portion of the threadmill.

[wojtek90]

I am trying to speed up process .

I have 200 parts and probably more in the future so making it in one OP would be more efficient . I think. 

[gcode]

50 minutes ago, wojtek90 said:

I am trying to speed up process .

I have 200 parts and probably more in the future so making it in one OP would be more efficient . I think. 

Put a junk plate in a vice and try it

I think you will change your mind

or

A simple test..

launch the Camex threading wizard and program a 3/4-NPT hole with a the tool I recommended and then with a single point tool

using the suggested feeds and speeds and default passes

Compare the cycle times  

[#Rekd™]

3 minutes ago, gcode said:

Put a junk plate in a vice and try it

I think you will change your mind

Doing it upside down will end up taking longer as he will most likely be hand tapping these to gauge them to size.

[wojtek90]

Ok. I will try do test. 

Taking out part from vice and flip them and put them in the fixture for taping  and remove them will take about 2 minutes !!!!!!!

[Colin Gilchrist]

1 minute ago, wojtek90 said:

Ok. I will try do test. 

Taking out part from vice and flip them and put them in the fixture for taping  and remove them will take about 2 minutes !!!!!!!

Do you have 2 vises?

Setup G54 work offset for Part 1 (top), and setup G55 for 2nd side Operation on part 1. (Tapping.)

Modify the program to machine all features on the Top side at G54, then tap and Deburr at G55.

Set G55 Operations in your NC Program with Block Skip. That way you can run the 1st part "once". After cutting the first part, you now have a piece to load into the G55 station.

Each time you open the doors to load a part, you first take the part in G54, and move/flip it to the G55 station. Then you load a new block of material in G54 station.

Doing this is called one-part-flow. Each time you press Cycle Start, and the program finishes, you have a finished part coming off the machine, and a new block of material going in...

[wojtek90]

Thank you for advice.  

Yes I have two vices. 

I will try to do this way.

  It still require to take out part from one vice and put it to second, but at least getting finished  part.

[Corey Hampshire]

One perk to the method Colin mentioned is the potential for reduced tool changes. If you use the same tool on both sides for machining, you can run it on both sides and save a tool change. This may not seem like a big deal, but all that time adds up over the course of a run. Just something else to think about.

[wojtek90]

Thank you. 

In my scenario  I only need run treadmill  on other side.  All features Blind and through hole as well as pocket I can run from one side. Only thread  because of direction of taper I will  probably  have to run on oposite side.