I’m trying to make a mount to hold a ball nut, the thread is 15/16"-16 and I ground an old 3/8"-16 tap so it only has one row of teeth left on it. I was trying to use it to thread mill and Sheetcam tells me there isn’t enough available room.
I have programmed this tool before manually and it works fine, so wonder what I’m doing wrong here. Support file attached.
I could just write it as a contour operation and go in and add my Z .0625" rise in the circle as it mills, but then I wouldn’t know how to use the threadmilling in SC… 
In your tool definition you need to change the thread depth. This is the distance from the crest of the tooth to the root of the tooth. This value depends on the pitch of your thread and the thread profile. At some point I must add a caclulator to assist with working this value out.
OK, I got it now… should this be the theoretical sharp corner to sharp corner value? Or the major diameter minus the minor diameter divided by 2, which is based on my drilling the minor for a 75% engagement thread?
Sharp corner to shard corner is .054125", the the amount based on major-minor divide by 2 is .03125"
Also, while we are talking about this, I usually in the past, start my thread mill at the bottom of the hole, climb cut CCW and rise one pitch to accomplish the complete thread (when you have a multi-rowed tooth profile). How would I accomplish that, and I noticed it asks number of teeth, is that vertically?
The formula would be a value specified for V-angle (we’ll assume 60º in this case) and the pitch, and then the formula would be pitch divided by 2 then times that by the cotangent of the (thread angle divided by two).
So .0625/2= .03125
.03125 x cot 30º (1.732)= .054125
Strictly it is the distance from the tip of the cutter tooth to the root. It is used to work out the cut depth.
The radius of the final tool path for an internal thread would be (hole radius + thread height) - cutter radius. For an outside thread it would be (boss radius - thread height) + cutter radius.
From: Brian L <blamb11@cox.net>
To: problems@forum.sheetcam.com
Sent: Monday, July 2, 2012 10:07:19 AM
Subject: Re: Thread milling question
Pardon my stupidity but how does one thread mill with
Sheetcam.
This means three axis all going at once??
Brian.
-------------------- m2f --------------------
Yes, the thread milling operation produces a spiral tool path to generate the thread.
Thanks Les, I reprogrammed it and using the sharp corner to sharp corner method the programmed path of the center of the cutter jives with what I had used before when I manually programmed it. I like that it calculates the Z ramp in the infeed and outfeed also, never bothered with that manually.
The one issue I do have is getting it to cut down in the part… I tried setting my zero setting deep (Z-.85) and then couldn’t figure out what to set the depth at… tried one pitch less, tried zero… all I could get is for the thread mill to go to Z0 in the code, then it ramps Z plus as it spirals around… which is what I was after, so I just changed the numbers for z by -.85 and that appears like it will do what I need.
To the other Brian… if your machine is capable of 3 axis simultaneous interpolation (which most have been since the mid 70’s), then you can use a tool called a thread mill and machine threads to any size and pitch. You use one with just one row of teeth to do many different pitches… like this one:
http://www.abtoolsinc.com/prod/thread-mills/
or you can get them made with many rows of teeth for a specific pitch, like these:
http://www.threadmillsusa.com/
Or, like in my case, I took a 3/8"-16 tap and ground away three of the four flutes, relieved the backside of the remaining flute a bit, and put it in a holder like an end mill and use it as a multi-tooth thread mill… not as good as one made for it, but for the oddball one or two parts, it gets the job done.
Set start depth to the top of the thread and cut depth to the bottom of the thread.
The direction depends on the ‘climb cut’ and ‘left hand’ check boxes. If both are off it spirals down clockwise. If climb cut is on it will spiral up counter clockwise. Turning on ‘Left hand’ reverses everything to give a left hand thread. Confused yet?
Got it, and it makes perfect sense once you tell me that the climb will set it for deepest first and come back up.
While we are talking thread mill, if I told it the tool only had 1 tooth in the tool definition, would it go deep and make continuous circles on the way out until it reaches the top? This would be good for a single point tool.
Yes a single point tool (1 tooth) will spiral for as many rotations as needed.
Les,
Another question in regards to thread milling… I should have asked when I was dealing with the above issues. Does SC have any provision for thread milling NPT threads (tapered pipe threads)?
I would prefer to use a single toothed cutter as each pipe thread is a different pitch. I do know they make multiple flute (full form) thread mills specifically for pipe threads, but it would be expensive to have the different sizes covered.
Also, it would seem that even with a tapered thread mill, you would have to program a slightly increasing circle (like a spiral instead of a circle) as you climbed in Z (assuming I’m starting at full depth). So I was wondering if I’m doomed to taps or whether SC will do tapered threads.
Currently SC will only do parallel threads. I had not even considered taper threads. To correctly generate the paths for a taper thread SC would need to generate a spiral helix. You can’t do this with arcs so it would have to be a series of short line segments. As long as the lines are kept short this shouldn’t be a problem.
I’ll add it to the do-do list but I am afraid I cannot guarantee when it will be implemented.
Hi Les,
Thank you for the answer, just wasn’t sure if it was something I was missing. I did some searching on the net, found tons of spreadsheets and software helpers that would/will do tapered pipe threads, but most are still for using tapered form hobbs and they only go in one circle, well, actually one spiral.
Some of the examples just do four quadrants, others have the option to break the spiral into as many sections as you like. I did find one macro listed that claims to be set up to do tapered threads with a single point tool, here is a link to a webpage with the information:
http://www.cncci.com/resources/tips/taper%20thread.htm
I don’t know if that would be helpful in adding the tapered thread ability to SC or not. My shop is currently switched over for wood production and I can’t get to my CNC mill at the moment to try it out (I have to move all my “stuff” on wheels to allow access to my panel saw).