Using joint between a component and threaded hole

[pkw6X2K4]

A component might have thread holes to which you want to fix another component. In such a case (generally) I will only wish to see the added component in position to check that the threaded hole is in the correct position. 

The added component will have a hole by which it will be bolted to the threaded hole in the mother component. If you use the join or align 'tool' you can set up the hole in the added component, because it is a simple  hole but it is not possible to to find a position to 'fix' the threaded hole because it is not a simple circle - it does not have a centre for the for the join or align  tool to engage with. 

Holes only join to holes  - holes do not join or align to threaded holes.

The question is: Is this true or am I missing something?

As always, I am grateful to the feed back from the community.

Thank you,

p.k.w

P.S.

In the past I have extruded holes and added a thread as I could suppress the thread to make a joint. But if you

have a hole operation that includes a thread it must be the intention that you can join something to it.  

[davebYYPCU]

What Geometry did you use to place the thread?

Use it to place the flange.

[pkw6X2K4]

Hello,

Thanks for your reply.
Excuse me if I do not understand your question
Here is am example;

A plate with a threaded hole made using the Hole tool
I have inserted another component into the workspace to join to it.
As you can see the have selected competent 1 but I cannot select component 2 the threaded hole.
This is my problem.

p.k.w

[davebYYPCU]

Nothing to see yet.

How did the hole tool know where to put the hole?

[pkw6X2K4]

Sorry, added screenshot

p.k.w

[davebYYPCU · Accepted solution]

If the threaded hole was not there, how would you otherwise place the joint?, 

selecting the top face will give you snap point in the centre of the face.  

If it were me, I would snap to the sketch point that you used for the hole and set the offset/s to the dimensions used for the hole.

That means if you used dimensions to place the hole, then those same dimensions will work for the joint offset/s.

[pkw6X2K4]

Hello,

So the answer is to turn on the sketch to show up the origin of the hole.

I did not think of this because when you use the join tool the surfaces of the components you want to
join a covered with potential joining surfaces and centres - the only one that is missing or cannot be located is
the centre of a threaded hole.

When the Hole tool was introduced this limitation could have been explained.
Of course, the problem already existed with extruded holes to which threads were added but the go around was to suppress the
thread in the time-line. The Hole tool is better than extruding a hole then threading it - except you cannot Join to the holes without adding the
sketch to the model to provide an origin. I suppose this is because the threaded hole is not a simple circle.

It’s just gone midnight here in Switzerland - - it is nice to end the day with a problem solved.



Many thanks,

p.k.w

[tomjulier · Accepted solution]

Do you have "modeled" checked for the threads in the hole feature? With modeled unchecked the hole remains a hole and I think you could check modeled again after the joint is created.

[pkw6X2K4]

Hello,

Good morning - not sure if it is morning where you are.

Yes, I check modelled.
I will take up your suggestion as soon as I have finished some work in a couple of hours.
So, excuse me if I cannot confirm this method right now.
But I guess you have already tested it or work with it.

I do not know if the reason that this problem exists is because a threaded hole
does not have a circular profile to connect with. No one from the Fusion team has
commented. Ideally, if you have a good program for modelling thread holes
it would make sense to be able to join things to them directly……..?

Many thanks and hopefully I can click your suggestion off as a solution!

Best wishes,


p.k.w

[tomjulier · Accepted solution]

As I see it, you want the threads to be modelled if the part is going to be 3D printed (for example) or for rendering, otherwise it's unnecessary, uses resources, and makes subsequent CAD/CAM more complicated. As you say, a cylindrical hole is no longer a cylindrical hole if you cut threads into it.

Using the sketch for joints and CAM is fine too though.

[pkw6X2K4]

Hello,

I still have not been able to get round to your suggestion (turning off modelling).
But you raised a good question for me.

I am not 3D printing.
I am modelling designs from which I make .step files and 2D drawings to send out for CNC machining.
This is the main purpose.

However, it might not be best practice for them to be modelled in the 2D drawings where the details of the holes and threads are, in any case, annotated.
I will check this with my engineer but I cannot see screws threads drawn in the ISO norms manual.
Therefore, from this point of view, it could be the case that I should not be modelling the threads at all.

The modelled threads look realistic in rendering or animations, which I also make of every design I produce.
So I have got into the habit of adding them.

Thank you for the insight.


p.k.w