topic Re: CREATE THREAD command creates the wrong threads in Fusion Design, Validate & Document Forum

CREATE THREAD command creates the wrong threads

russtuff — Wed, 09 Nov 2016 04:06:19 GMT

This must be a new bug, but I can't find someone else having mentioned it (admittedly, I'm bad at this site).

I have a program with some 10-32 holes, and I've CAM'd them correctly before. Today I reposted some gcode and where I hectically interpolated some #10 holes, they ended up being #8 holes. I took some screen shots, see below.

Also, when I intentionally try to make a #8 it becomes a #6, and if I try and make a 1/4" thread it's coming out at .2014" diameter.

For tonight I updated my model so the holes are 12-32s and they are measuring like a #10 so at least I have a workaround for now.

Re: CREATE THREAD command creates the wrong threads

TheCADWhisperer — Wed, 09 Nov 2016 12:45:18 GMT

I just tried 8-32 10-32 and 1/4-20 using both sketched holes and using the hole command.

Then added the threads.

The tapped drilled sizes were correct.

Can you attach example where the holes are incorrect?

Re: CREATE THREAD command creates the wrong threads

HughesTooling — Wed, 09 Nov 2016 13:44:55 GMT

It does seem do something odd if the start hole is not the correct size, it seems to default to #10 if the last thread added uses the wrong size start hole and the thread you're editing used the wrong sized start hole. All seems Ok if you make the holes 0.16" to start with. The hole in the part is made 0.1601 as that's the correct size the #8 that's shown on the dialog (0.164) is just a suggestion as the closest drill.

You can check the thread data here.

http://www.amesweb.info/Screws/TapDrillSizesForUnifiedScrewThread.aspx

Mark

Edit I don't use UNF or number drills, in the UK a #8 drill is 0.199" so is that wrong as well?

Edit 2. I should have said it defaults to #10 if the last thread added uses the wrong size start hole.

Re: CREATE THREAD command creates the wrong threads

TheCADWhisperer — Wed, 09 Nov 2016 14:20:22 GMT

@HughesTooling wrote:

... number drills, in the UK a #8 drill is 0.199" so is that wrong as well?.

In the US the OD of a #8 drill is 0.199"

In the US the OD of a #8 fastener is 0.164"

The tap drill size for a #8-32 thread is a #29 drill (0.136) (more or less depending on desired fit).

The correct tap-drill size for a 1/4-20 UNC is a #7 drill (0.201).

Re: CREATE THREAD command creates the wrong threads

Mike.Grau — Wed, 09 Nov 2016 14:31:19 GMT

Hi @russtuff,

Thank you for pointing to that.

I could reproduce what you have described in a similar way.

It would be great if you could share your design with us?

Thanks,

Re: CREATE THREAD command creates the wrong threads

HughesTooling — Wed, 09 Nov 2016 14:39:05 GMT

Thanks @TheCADWhisperer

So this is right for a 10-32 UNF thread, this is what I get if the start hole in the body is 0.160

But if I add a couple of holes at 0.2 then add a 10-32 thread it reports the wrong size when I go back and edit the first.

Mark

Re: CREATE THREAD command creates the wrong threads

JDMather — Wed, 09 Nov 2016 16:26:54 GMT

The operator must pay attention to setting all of the variables in the Thread dialog box.

Size of fastener (Fusion will adjust the tap-drill hole as needed).

The pitch of the fastener (Designation).

Class of fit.

Direction R or L hand helix.

For example, it is common for a beginner to create a .25 hole for a 1/4-20 UNC thread.

But .25 is not the correct tap-drill size for a 1/4-20 thread - there would be no material for the thread. The fastener would slide through the hole if pushed or pulled.

The minimum diameter is .201 (more or less) for the helix to be cut into the hole.

So if the beginner mistakenly creates a .25 hole and then specifies a1/4 fastener Size and 1/4-20 thread pitch Designation - Fusion automatically adjust the hole to correct size.

Re: CREATE THREAD command creates the wrong threads

HughesTooling — Wed, 09 Nov 2016 18:09:04 GMT

@Anonymous wrote:

So if the beginner mistakenly creates a .25 hole and then specifies a1/4 fastener Size and 1/4-20 thread pitch Designation - Fusion automatically adjust the hole to correct size.

Although it corrects the size if you go back and edit the thread, in the case of a 10-32 unf thread it sometimes reports the Size as 0.164"(#). The fact that it's not consistant should be investigated.

Mark

Edit. I don't work in inches so I've just experimented a bit in mm. Working with mm it all seems to work correctly, never really thought about how the dialog worked before because it always worked correctly. I see now the size is the fastener OD so for 10-32 Size should always be #10, when it reports #8 it's wrong. Also see now the hole tool expects you to make the start hole the OD of the fastener, it seems to get confused if you make the hole the tapping size.

Re: CREATE THREAD command creates the wrong threads

JDMather — Wed, 09 Nov 2016 19:30:52 GMT

@HughesTooling wrote:

...the hole tool expects you to make the start hole the OD of the fastener, it seems to get confused if you make the hole the tapping size.

The key is that Fusion has to make a decision and there are two possible inputs 1. the Thread OD. or 2. the Tap Drill Size.

The nice thing is that if you fill out the Thread dialog correctly - Fusion corrects your hole either way, but it can't make that decision for you in either case, only in the one case.

Now the way it should really work is -

the Hole feature should include Thread option when creating the hole instead of it being a secondary feature. But that still wouldn't stop the beginner from using an Extruded circle for holes.

Maybe someday when Fusion includes fastener library.... .... it will become more apparent why Holes should be created as Hole features rather than as Extrudes. Sounds like a good idea (or two) for the IdeaStation.

Re: CREATE THREAD command creates the wrong threads

russtuff — Thu, 10 Nov 2016 04:52:01 GMT

I have duplicated this issue in another model, which you can access here: http://a360.co/2fEeB21

It is the same model I took screenshots of in my first post. Sorry, I'm not going to post/share my fixture where I first came across the issue.

I have machined clearance holes for screws many times using the exact method I described originally. The fixture model I used is the same one I've been using for over a year and when I select the tapped hole diameter for machining the clearance, it has always worked. I'm not saying it was right or wrong before today (or today), but something has definitely changed. If (going forward) I need to create a hole feature prior to a thread feature then I'll change my process.

I appreciate everyone's help.

Re: CREATE THREAD command creates the wrong threads

JDMather — Thu, 10 Nov 2016 14:40:24 GMT

@russtuff wrote:

I have duplicated this issue in another model, which you can access here: http://a360.co/2fEeB21

....

I could not find anything wrong in the file that you linked.

All looked correct to me? Can you state the exact issue with that file?

You state "clearance hole", yet you posted a threaded hole?

These are two entirely different things.

Here is an image from Autodesk Inventor that does both Clearance Holes and Threaded Hole types for fasteners.

Re: CREATE THREAD command creates the wrong threads

Phil.E — Fri, 11 Nov 2016 18:08:01 GMT

All,

Thanks for your input and discussion. Let's sort this out.

The short answer is: there is a bug in the Edit Thread dialog that lists (in this example) #8 Ø.164 as the "size". That is wrong. I can easily get this by creating a #10-32 UNF threaded hole and then just edit the thread a few times and Fusion will eventually show the #8 instead of #10 for nominal size. If you measure the hole with 10-32 UNF threads, no matter what the edit dialog says, the measure is Ø.160 which is a good tap drill size for 10-32. I'm logging this as a bug against the edit logic. I think there must be a tolerance issue when it's trying to decide what to show for nominal size.

Regarding the dialog and why it's confusing here:

The "size" field in the dialog is only nominal, not tap drill.
It is used in the Thread workflow to pick a range of threads.

Intended steps to utilize Size variable:

1. Starting with any size plain hole in a part.

2. Start Thread command

3. Pick the cylindrical face to thread

4. Pick the size from the size dropdown

5. Pick the exact thread from the available range of threads for that particular "size".

SIDE NOTE: One of the most awesome things Fusion does for you is in this workflow. It may be entirely unique to Fusion. You can import any generic STEP file, with any "drill sizes" for the holes, and apply whatever thread you want!! Fusion will resize the holes for you. I don't think any other CAD does that, including Inventor. You can go from generic import, to perfect threaded holes, in just a few picks. The thread command will alter any regular cylinder (within reasonable limits according to the model geometry) to match the thread you callout. It provides the nominal tap drill size for the actually modeled hole, just in case you send the model directly to CNC.

Thanks,