HOLE WITH THREADING OPTION

[Farzati.Scott]

First of all kudos for putting such a feature together.  Saves time and have found it simple to apply threaded holes all at once.  However there may be some review needed so that tap sizes correspond correctly to the drill size.  I am attaching an example of a #8-32 2B tapped hole.  The drill size and hole it makes is .1345 without the option to change it.  Firstly that is not a standard drill size.  The proper sizes would be #30 for 75% of thread, #29 for 70% and #28 for 60% accordingly.  Not sure what would be involved to remedy this?  75% is most common.  I'm sure you are using some sort of mathematical calculation.  However, it is important to be applying the correct sizes when doing real world blueprints and cam applications.  This may also have a impact when countersinking for the thread??

[Farzati.Scott]

I just looked at thread data for a #8-32.  Appears it is taking the minor diameter for the thread which is what the tap cuts.  However this would not be the actual drill hole size that would be required...

[paul.clauss]

Hi @Farzati.Scott

Thanks for posting - this is working as intended. Fusion 360 will currently adjust the diameter of a threaded hole to the minor diameter of the thread. There has been some discussion about this in the past and I would recommend giving this Ideastation post a vote or comment if you'd like to see this changed in a future update.

My two cents on this issue is that, as long as the hole center is in the right place, you just need to be sure to drop the correct drill and then tap into the hole during manufacturing - regardless of how the hole is modeled. I can see arguments for this being shown in Fusion either way and the Ideastation will be the place to discuss any potential changes with the dev team.

[Farzati.Scott]

I agree that you can easily drop any size drill into the hole. However, I
don't agree that the hole size should default to the minor size of the
thread. Seems it was just a easy work around. When tapping or
threadmilling the size of a threads minor varies depending upon the % of
thread desired. Nominal of the specifications that are listed for the
minor are not relevant so to speak. This is the reason why tap drill
charts exist. Would rather see it incorporated like the team at Fusion did
for the "Counterbores". Close, normal and loose fit respectively. This
could also be applied to tap drill size with the percent of thread desired
being real world drill sizes. Think its fantastic that so much attention
is given to the design of models and their functionality, but just as
important is the application with CAM and posting to the machines for the
production not just design. It is easier to reference hole sizes for tap
drills at any given time by doing a inspection of the hole to be threaded
(can aide in catching errors). Guess I can continue to use the hole
feature without applying threads & do it as a separate function. Nice
feature, but if the need to verify in CAM is not available then don't see
much use for it if I want to apply the correct size hole to my thread.

[paul.clauss]

Hi @Farzati.Scott

Thanks for the response. I agree that, from a manufacturability standpoint, having the option to define percentage of thread desired would be a great option. Please post this idea on the Fusion 360 Ideastation - you'd have my vote.

One way to approach easily defining the parameters for these holes in the CAM workspace could be to use CAM Templates. NYCCNC has a great video on templates here as well. You could create different templates for each thread and percentage of thread desired - this could make the workflow more efficient.

[Lonnie.Cady]

There is more to it IMO.  I just started using it and changing the thread pitch from a 5/8-11 to a 5/8-18 has not effect on the holes size even though the minor diameter would be different in this case.  It really should model to the drill tap size and allow it to be overridden if needed.

I think from a drawing and manufactuing stand point SW has it pretty good.  You can set it to have the tap drill modeled at the correct diameter and the tapped section modeled to the major diameter.  It provided much greater clarity about what is intended.  From a CAM standpoint you can select the one face for your drill depth and one for your tap depth vs manually having to set the correct tap depth manually in the operation which will not update if the tapped hole depth changes and completely goes against the basis of having an integrated cad/cam.  Also works well for driving a thread mill to the major diameter.