Tapered threading, cutting counterbore

[christopher.leblanc]

  Ok, will try to explain the easiest way I can.  Cutting a 3 1/2 IF Box,  Which is a 4 TPI .250 pitch .119 deep.  When threading it always cuts into the counterbore which It shouldn't touch the counterbore.  I moved the offset to .1 from where it is suppose to start cutting which it does look correctly except and I could be wrong, the start point as it comes in cuts a circle on the first thread then moves forward in lead.  I have done this 1000's of time on Mazak using Mazak program pulled the same numbers for my model in fusion and it still cuts into the counter bore.  I am sure the pathing is the same on pins, you j just can't see it because the pins threading starts at the begging.  Is there a way to make it thread coming in straight and then taper up from the spot it is suppose to start to the end rather than start tapering from the start of part?  Hope I explained this clear enough.  Included print if someone has the answer.

[seth.madore]

In Threading, there is an option for "Helical Leads", this will have the effect of cutting lower or higher than specified. Is that the case here? Would you be able to share your Fusion file here?
File > Export > Save to local folder, return to thread and attach the .f3d/.f3z file in your reply.

[christopher.leblanc]

Sure, I think my probably has something too do with the tool and insert not being described correctly.  The Lathe is down atm waiting on a part to come in so I can't test it, but here is the 3 1/2 IF Box.

[christopher.leblanc]

Here is the updated tool info not sure why it didn't export with the correct thread bar on the first one, but its still cutting the counterbore in the simulation

[seth.madore]

Ah, didn't realize this was a Turning toolpath, so disregard my prior comments about Helical Leads.

Looking at your Sketch, are you certain that all the values are correct? Your Sketch is unconstrained (all blue), so it's telling us that features haven't been defined thoroughly. Some of the dimensions you have on the sketch are not present on the PDF that you shared, so I'm curious what your source of them are 🤔

Point of clarification: the counterbore you're referring to is the front tapered bore, correct?

[christopher.leblanc]

They are accurate I did different versions between an older rotary connection, gage maker and older programs. Every setup does the same thing, I am thinking it has to do with the tool in the library missing something because everything but the threading comes out perfect every time. Fusion should get on the ball with this, mill work everything works fine on every mill on have setup but when it comes to threading internal tapered threads everything seems to goto **** and so little info on this. Trying to stay with fusion but it’s getting to the point where I have to make a decision to stay with this or just switch to Gibbscam.

[a.laasW8M6T]

Hi, I'll start off by saying that I know nothing about API connections but,

Are you sure that its modelled correctly?

If you draw a line .119 away from the ID you can see its deeper than the counterbore

Which pretty much matches what your seeing the threading cycle do in Fusion

I cant find any good dimensional data for that connection online.

[a.laasW8M6T]

Hi

I missed there was a Drawing in the First post.

From what I can gather from that drawing although it doesn't have quite enough info like Seth says, you haven't modeled it correctly.

You have 5 degrees for the thread taper but from what I can see its 2"per foot taper included angle which works out to 4.73°.

I also don't see any mention of the 10degree taper in the Counterbore, that appears to be the same as the thread angle.

I have re modeled it to what I think are the correct dimensions and you can see the thread doesn't hit the counter bored area, again I don't know anything about API connections so could be completely wrong

Also everything is at nominal dimensions, no allowance for the tolerances there

See attached file

[seth.madore]

@a.laasW8M6T man, thanks for jumping in. I was extremely sleep deprived yesterday (16hr road-trip in one go) and my brain was in a fog. I was scratching my head trying to make sense of the print and correlating it to the model. I went down the rabbit hole of API/IF connections and it looks like a lot of the data is hidden behind paywalls. I, too, was not seeing a lot of the data represented in the Fusion file.

[christopher.leblanc]

   I really appreciate all the input, and I do apologize Its been a very very long week.  I've had the owner of the company in the way and quite literally standing over my shoulder for months now.  While I know he just wants to understand how a Cnc lathe, programs, and a million other factors.  Fusion 360 is 100% self taught, and while I'm quite good at using it for mill work for last 2 years.  I have never been so frustrated in my life when it comes to the little data there is on doing the simplest things on a lathe, and maybe it's just a bad fit for using on a lathe.  This is the first Milltronics machine I have ever touched and in 25 years of programming, setting up and running laths/mills its by far the biggest POS I have ever seen.  They defiantly took advantage of him not knowing anything about CNC's and sold him something that just doesn't function in the norm or very well at what it does.

  Back to the problem at hand,  What I did was took an old 3 1/2 IF box program and drew out the connection point to point.  As well as used a scaled print to measure the angles and triple check them on fusion as I drew them out.  The degree's vary here and there by a degree or two over time from the tolerances changing or dimensions for whatever reason being changed.  Even the old programs drawn out cut the counter bore in fusion but not on the actual CNC running it.  This is what is driving me up the wall thinking it's got to be something with the way I defined the insert and bar.  I setup and program a pin it comes out perfect, boxes always cut into the counter bore.  I even took a repo mold of an older connection already cut and compared to the repo of one I cut last week and the angles line up.  I know there isn't that much of a visual difference at first between 5 degree and 10 degree but those are the numbers from  the older program ran in 2015.  Now I Was't there back then to say 100% if they were just saying forget it and cutting into the counter bore or not, but I can take print off pagemaker or the rotary book goto a Mazak and program it out perfect every time.  Just at a loss right now, and while I of course could fake it with 5 degrees on the counterbore and I am sure the inspectors wouldn't catch it, sooner or later someone will and I believe in doing things the right way.

Sure don't want to be the one the finger is pointed at for bad machine work if there ends up being another BP oil spill and comes back to the degree on the connection was off 5 degrees.

[seth.madore]

---

@christopher.leblanc wrote:

   I really appreciate all the input, and I do apologize Its been a very very long week.  I've had the owner of the company in the way and quite literally standing over my shoulder for months now.  

---

Oh man, I've been there (also a machinist/programmer of 25 years), certainly not fun or conducive to learning.

---

@christopher.leblanc wrote:

     Back to the problem at hand,  What I did was took an old 3 1/2 IF box program and drew out the connection point to point.  As well as used a scaled print to measure the angles and triple check them on fusion as I drew them out.  The degree's vary here and there by a degree or two over time from the tolerances changing or dimensions for whatever reason being changed.  Even the old programs drawn out cut the counter bore in fusion but not on the actual CNC running it.  This is what is driving me up the wall thinking it's got to be something with the way I defined the insert and bar.  I setup and program a pin it comes out perfect, boxes always cut into the counter bore.  I even took a repo mold of an older connection already cut and compared to the repo of one I cut last week and the angles line up.  I know there isn't that much of a visual difference at first between 5 degree and 10 degree but those are the numbers from  the older program ran in 2015.  Now I Was't there back then to say 100% if they were just saying forget it and cutting into the counter bore or not, but I can take print off pagemaker or the rotary book goto a Mazak and program it out perfect every time.  Just at a loss right now, and while I of course could fake it with 5 degrees on the counterbore and I am sure the inspectors wouldn't catch it, sooner or later someone will and I believe in doing things the right way.

Sure don't want to be the one the finger is pointed at for bad machine work if there ends up being another BP oil spill and comes back to the degree on the connection was off 5 degrees.

---

Do you have the paid access to the API thread specs to confirm that the numbers you're using (in your original file) are valid? Everything I found on the 'net was missing some critical info and leaving it to assumption (and you know what they say about assume...)

[a.laasW8M6T]

Hi, sorry if it seems I'm being a bit stubborn here but,

I would be pretty wary of trusting old programs, I've looked at old programs people had at work for Cutting BSPT threads and they were waay off, I got the correct data from the standard an re wrote the programs and checked them with the thread gauges, not that BSPT is particularly critical in our applications

When I used to make JIC fittings for Liquid Ammonia connections I made the company Buy the ISO standard so they could get all the dimensions correct as they had just been fudging it before.

Looks like the API or Iso standard for these is only like $200 but you say you have print from Gagemaker software or another source, can you share those?

From all the information I am able to gather based on various excerpts from the standards online that aren't behind a paywall

there are some Key dimensions to consider

• Counterbore Major Diameter 4.078, you have that correct
• Thread Pitch Diameter 3.808 at 0.625 back from the front face, Your sketch doesn't fit with that dimension
• Thread height above pitch line 0.07
• Thread taper is 2" per foot AND thread taper = counterbore taper according to this from ISO 10424

so 2/(arcTAN(2/12)) = 4.73116°

Video with some tips on getting a fully constrained sketch for the revolve

File attached with corrected dimensions, I didn't realize the 3.808 was the pitch Diameter in the first one I shared

[christopher.leblanc]

  Wanted to thank every one for the time and patience.  While I still have a lot to learn drawing up the models I worked through it.  The videos and models supplied helped 100%.