Thread milling help

Ok, so trying to figure out the thread mill path in V24. Currently trying to cut 1 5/16" -12 threads. I have the hole size, put in the thread diam size, thread pitch (.083) and what I think is the right thread height (.040). Once done my fitting will start in it but feels like its too much interference. It seems like no matter what I try it will not cut the threads any deeper. I can go from .040 to .200 and it will cut what seems like the same exact threads. Not sure what else to try other then making the dia. size bigger but really dont want to do that.

Thanks.

I do not have the time to look right now,BUT,,down and dirty,tell the software you are using a smaller tool than actual.It is like cutter comp in a way.It will work,I did it Monday on some parts running V23.

I looked at your file,but I had to look at it with V25.I have 23,25,and 26,but no 24.
One thing I did not see was a point.For center drilling,drilling holes,tapping,threading you need not draw the arc(hole),just use a point in the center.
The way I thread mill is I enter the data at "Nominal" values and "mean" values.

Outside is 1.3125
Minor at1.222
Thread Height = 1.3125 - 1.222 = .0905 / 2 = .0452

Now,one could say the thread height is slightly wrong,and I would agree.Because of the little details of correct thread form with the radius on the root and,blah,blah,,,,BUT,this will get you close.From here I dial it in by changing the tool diameter.
Now I did ask for a picture of your tool.There are different kinds and that will make a big difference.
Wish I could share a file,but I have no 24.

BTW,I would use 4 decimal places with the pitch.The longer the thread engagement,the more critical this will become a factor. .0833

It wont let me do that many decimal points? I have tried but it wont hold that many and rounds alot of times. Assuming I need to change a setting somewhere for that.

This is like what I am using, https://m.mscdirect.com/mobileweb/pr...tedParts=false

Go to preferences/default/units

Your tool would be a single point so entering 1 for threads per revolution is correct.

Here is a simulation of your exact thread in V26.
This is the standard simulation that comes with V26....V27 is pretty much the same.
Quality goes down with video recording at the same time
but
although not %100 accurate all the time,,it is pretty darn close,,,,what you see is what you get.Real handy here when your struggling with a tool path.I am probably not spot on,,,there is just too many little tiny things that come in to play that determines final size(not to mention poorly ground tools).But I think this should be expected.Ever make threads on the manual Lathe ? same thing.But I can see I am not far off.Dial it in little by little.Like I say,I like to just change tool diameter a little at a time.I am usually within .004 at most.
I probably should of made the hole.005 to .01 larger so the threads were not so sharp,which would be perfectly OK as far as tolerance goes.

https://www.youtube.com/watch?v=wtJK...ature=youtu.be

I get changing the tool size but why should I have to? Just the variances in tool shapes? Seems like it should cut exactly what I input and not have to do work arounds which it seems like I am constantly doing, some because I dont know the software well enough yet and some because that is the only way to make it work. Gets frustrating.

Thank you very much for the help though. I am gonna try and beat up a BCC sales guy and see how much they can get me into 27 for and a lic transfer. Dolphin is trying to sell us 2 seats of mill/lathe for 750 bucks. Seems like a lateral or less then lateral move though.

Well for one thing,did you notice how my numbers and your numbers are a little different?
Tool spring another cause of .001 or so.
All cutting edges of tool not equal lengths and/or concentric to the center shaft.
Run out from your tool holder and machine spindle.
Concentricity and positioning from one part to the next.
How accurate your machine is.
Material to be cut and what you select as speeds and feeds.
Coolant that you use.
Rigidness of set-up.
How you are measuring and qualifying your tool dimensions
Where are you getting your numbers from ?? Machinery Handbook would be a good source.
.001 TO .002 is all it takes to ruin your work.
Threads are by far the hardest single thing that you will routinely do.
I do not know your knowledge of threads.But I still am learning pieces and parts.I have made thousands and thousands.A lot of the threads I make are 3a or 3b.Sloppy old threads are not exceptable.Getting the first article done within .003 to .004 is reasonable to me.It is part of the set-up.I do not see how any software can do any better in.this area.There are little tiny things that simply make nailing it not reasonable.

Ok makes sense. I have never made threads before other then taps. I can see how just a slight difference in tool shape or size can greatly effect the outcome. Where my newbness shows is I want to blame the software for making me do work arounds with something that needs to be .001 precise but in reality its just nature of the beast.

On a good note, changed my tool size -.015 and my fitting threads in perfect! The biggest issue with how its done is I dont have the verify setup like you so only way I can see the outcome of the threads is to actually thread it in something. We were using a piece of plastic but it looks like Swiss cheese now lol.

Threads can be one mans whole career.You start getting into J threads,Trapezoids,MJ threads,British,,,the list is very long.Luckily the Unified is very easy.If you are going to be doing any precision work,you need some basics at least on threads.Machinist Handbook is one such source.

"On a good note, changed my tool size -.015 and my fitting threads in perfect! "


did you notice my thread depth was .0052 deeper than yours ? That would be .0052 X 2 = .0104.I am within .0046 right off the bat.And the good thing is the part is not scrap :)
Machinery Handbook is where I got the minor diameter from.That in return affects your thread height calculation.

I always add a g41 to the code so I can adjust size at the machine.