Taper Threadmilling

[rmsmachine]

I was wondering if there is any capability in Fusion 360 CAM to threadmill a tapered thread.

We have some parts that have larger NPT threads that we threadmill but I do not see that as an option.

Am I missing something?

Thanks,

RMS Machine

[Steinwerks]

Are you using an NPT thread mill or a single point thread mill?

[rmsmachine]

NPT Thread Mill, not single point.

Thanks,

RMS Machine

[Steinwerks]

So you're correct that there is no tool type for this yet, but as a workaround you can create a tapered end mill that matches the basic dimensions of the thread mill, and there is a tool path for thread milling, it just won't simulate correctly.

[rmsmachine]

I am not worried about the tool type, I can come up with something there.

In order to properly thread mill a NPT thread you cannot do a regular thread mill operation.  You need to be able to input the taper angle so when the tool does its helix pattern it does so with a continually decreasing radius.

Now I say "properly" because if using a NPT thread mill you can get by with a normal thread milling operation but the form will have a small error in it that is easily taken up by thread tape or thread sealant. 

I would prefer the correct method.

Thanks,,

RMS Machine

[CGPM]

The current correct method, as far as I know, is to create a tapered plug as it's own file then import it to use as a subtraction tool to make your part geometry.  Don't try to model the threads.  Then just thread mill it in cam, I use an end mill of the correct diameter.  The tool will follow the tapered hole nicely.  I do this fairly often with a single point thread mill and works exactly as it should for NPT threads.

[cj.abraham · Accepted solution]

It is possible to create a tapered thread mill operation in Fusion. A tapered endmill is not currently compatible with the thread operation, so you will need to use the thread toolpath with an equivalent threadmill or flat endmill. Create a hole with a tapered face with the appropriate angle, and select that face for the geoemtry. This will create a thread toolpath with a taper that matches the selected face.

[rmsmachine]

Chris, thanks for the solution. 

It is not how I would do it, but I will do some test cuts and make templates so after that I should be good.

One note for future readers of this:  As I was trying this out I was using the thread milling function under the drilling menu.  That will not work.  You have to use the stand alone thread milling operation under the 2d operations section.

Thanks,

RMS Machine

[Anonymous]

i'm new, and spent lots of money on this software, isn't there an easier way, i only understand about 1/4 of the workaround

really, i spent lots of money and your competition software won't even tell me how much it is without filling out forms

is there a timeline on this?

i'm losing customers over this ya know

[cj.abraham]

All you need to do is model the hole with the proper angle and diameter, and the thread mill toolpath will cut the proper NPT thread.

Fusion, HSMWorks, and InventorHSM all do currently support cutting tapered threads.

[Lonnie.Cady]

@rmsmachine If you are using an NPT multi tooth thread mill you also don't need to spiral all the way out of the hole.

I mill a lot of npt threads and I set the bottom height at the bottom of the hole then set the top height to just slightly more than one thread pitch above the bottom height.  By going just slightly more than one thread pitch you will get a little overlap in the tool path.

https://forums.autodesk.com/t5/computer-aided-machining-cam/thread-milling-npt-work-around/m-p/55500...

here was an old video I did on it.  I would have thought the fusion team would have added tapered threads to the modeling side by now.  I created plugs that were the size of npt threads and stored them.  I inserted them and did a Boolean subtract.  Not the easiest way but at least you can reuse the plugs you make.

[tcgarcia]

I had created a tapered hole but the thread manufacture operation would not let me select the hole face (irregardless of tool selection).  I figured out the way the hole was created in the model was the problem.  I had created the hole by lofting between 2 hole sizes.  The "correct" way was to create the hole on one face and extrude  (cut) and enter a taper angle (negative if tapering smaller).  After I redesigned the holes, the thread operation let me select the hole face.