Modelling a female thread

[Anonymous]

Hi all,

I'm currently trying to model a part which will screw onto a telescopic pole head. I've got the rest of the part sorted, and ready for injection mould tooling, but have got stuck doing the thread. The manufacturer of the pole has given me a technical drawing of the male thread, and so I am trying to use this to model the female thread.

Non of the pre-defined threads in Fusion 360 come close to the thread I need. After much research, the closest thread I can find is an ACME 3/4-5 thread for which I can download the IGS file from here...

http://www.mcmaster.com/#95080a112/=14nl8db

I'm not sure that this is quite right though, and I wonder if I'm better just modelling it myself using the coil command.

I've attached my first attempt at modelling this and below is the technical dimensions of the male part of the thread that I am planning to use. I intend to get the part 3d printed first before having the tooling made for injection moulding.

Can anyone with more experience than me (virtually everyone!) give me any pointers please?

Thanks, Damian

[paul.clauss · Accepted solution]

Hi @Anonymous

Thanks for posting. It looks like you are trying to create a custom female thread that is not included in the default options of Fusion 360.

Firstly, nice work on your first attempt at modeling custom female threads! The model looks very good. 

A few thoughts:

1. There is a method to create custom threads in Fusion 360 that will appear in the "Thread" command. This is advantageous if you use custom threads consistently, as you can define the thread properties once and save the thread template instead of creating new threads with the coil command each time. This process is described at this link. Unfortunately, I do not think that this process will work for your particular thread because of the circular thread type (this method only supports trapezoidal, sharp, square, and Whitworth thread profiles).
2. In your "thread v1" model, you could clean up the top edge of the tapped hole by using a swept cut instead of chamfer. I have attached a screencast illustrating this below: 

3. Because you have the technical drawing for the male threads, it may be easier to approach this problem by modeling the male thread and then using the "Boundary Fill" command to create the negative space of the female thread. I have also created a screencast illustrating this process and attached it below:

Hopefully helps you create the custom female threads you need for your design! If you have any other questions, please let me know and we can continue troubleshooting,

Thanks,

[Beyondforce]

Hi @Anonymous,

You can also use this technique: https://www.youtube.com/watch?v=ulWdXl4X3oo

Let me know if you have questions.

Cheers / Ben
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[Anonymous]

Hi @paul.clauss,

Thanks very much for your really helpful screencasts. That's a really cool way of modelling the thread and I should be able to finish my model now based upon your help. I'm thinking that I may slightly scale the female thread up in size very slightly from the male thread to allow for tolerances in the injection moulding process. I don't think it'll matter too much if the female thread is very slightly too big, but obviously would matter if it's slightly too small.

I've only been using Fusion 360 for a few weeks just to create this model but this process has inspired me to try and learn the programme properly. I've managed to get it to do what I want but know that there's probably easier and quicker ways to do virtually everything that I'm doing.

Thanks once again,

Damian

[paul.clauss]

Hi @Anonymous,

I'm glad the screencasts helped! You are absolutely right - there are many ways that will work to create almost any geometry in CAD, but the key is figuring out which method works most efficiently.

I was also thinking about thread tolerances when I made the previous post, and wanted to share my method with you. You could also experiment with using the Split Bodies command or use the modeling techniques from my last post and simply scaling up the male threads.

Thanks,

[Anonymous]

Thanks once again @paul.clauss,

That's a much better way than the way I was planning to do it. I really wasn't expecting such a thorough and complete answer to my question.

Thanks again,

Damian

[HughesTooling]

As a mould maker\designer I found this thread quite interesting, haven't had time to post until today. Modeling thread lead-in\outs on moulded parts can be a bit of a challenge, also what's mouldable is pretty much opposite of what's machineable.

Here's an example of the core for your thread with lead-outs that can be made, left is thread ground right turned with a feathered lead-out. Screencast to follow.

Mark

[HughesTooling · Accepted solution]

Here's the screencast and file. I made a few small mistakes in the screencast.

First I should have created a component at the start.

Second I forgot the draft on the first extrusion. Edit Watching the screencast, looks like I didn't foget I just used a draft as the next feature.

Last, the battle with the sketcher adding a dimension to the line for the rotate cut, I finally beat it adding this line.

Mark

[Anonymous]

Hi Mark,

Sorry I was slow to find your posts and screencast. That thread looks amazing, I'd have never have been able to do that on my own. I've watched your screencast once but will watch it many times more to be able to understand it. The more I see of Autodesk, the more I want to be able to use it properly!

Many thanks, Damian

[Anonymous]

Hi @HughesTooling,

I've just followed your screencast and made the thread. I've learnt an awful lot in the process and can follow what you've done and why.

I've used the boundary fill method to make a cavity in the shape of your thread in the part that I am producing, and then to check if the male thread will fit, I've made a model of the male part of the thread as per the technical drawing above.

When I've inserted this into the female thread cavity, it looks pretty tight and begins to touch the female thread after only three or so turns. Is this intentional in the design to make it a tight fit, or should I add less draft angle / start the female thread model on a bigger spindle?

Here's a screenshot to show you what I mean...

Many thanks once again for your help,

Damian

[HughesTooling]

On threaded cores I've made I've never needed draft, pretty sure this would unscrew fine once it's all hot. I downloaded the file in the first post and followed the draft etc. from that, thinking about it more now the 18.2mm should have been at the small end and the 1.5 rad should have been 1.6, you'll need to reduce the cross section of the coil feature to 1.8 as well.

I'll reply to your PM in a minute and arrange a time for a call.

Thanks Mark. 

[Beyondforce]

Hi @Anonymous,

Here is another easy and simple way of Modelling a female thread:

Cheers / Ben
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