All information to draw this is in the drawing. The only difference from a normal thread is that the thread has a 'Taper'.  When constructing the thread, type in the 'Taper Angle' in the box provided. Make sure you change the 'Units' in File - DesignSpark Options - Units - Angle - to -  Deg/Min/Sec.

There are many tutorials on how to make a thread. All you need is the 'Triangular shape' of the thread. Placed in the correct position from the axis. Then 'Pull' this surface with the 'Rotate' option around the central axis, with 'Revolve Helix' option picked in the 'Revolve Options'

I figured out how to add the taper, while also adding arcs to make the chamfers. But now I do not know how to terminate the thread at the top or the bottom. any thoughts or ideas would be welcome

The easiest way is to 'Combine/Cut' the thread using a 'Plane'. This is best used on the inside of the thread not on the end.

Place an 'Axis' on the model to use a reference point. Place a 'Plane' and move it so it will 'Cut' through the thread. Combine/Cut the thread using the 'Plane' as the cutter. Select the cut end. Draw a circle to the original diameter on the end using the 'Axis' line as the center point. Pull this up to the original length. You may need to 'Taper' this using the option 'Draft'. Combine/Join if it has not joined automatically.

There are a number of ways you can finish the end i.e you could just draw a triangle to use as a cutter to cut the end to look like a 'chamfer'.

Looking at your model, You could Copy and Paste the profile of the end of the thread. Using the end of the Model as a new sketch plane. Move it to the middle of the pasted surface. Draw an 'Arc' from the new surface to make a gradual curve into the solid. This will have to be perpendicular to the surface because of the taper. Now 'Pull' the surface with the 'Sweep ' option to follow the drawn curve into the solid.

You could try this on the inside end as well.

I am having no luck being able to draw this. Mostly because I cannot get the bottom 45deg taper on the pin to work out. I know what they look like in real life and I cannot replicate that. Another reason is I am most certain I cannot read this drawing properly. What would a person need to do to get someone to make a video of drawing the pin end of the thread so I can see the procedure?

There may be an easier way to do this.

Copy and Paste the profile face of the thread. Create a new 'Sketch Plane' on this surface. Draw a line midpoint to midpoint on the surface.

Create a new Sketch Plane on the bottom, Move it upto the line just drawn. Move the 'Anchor' to the middle of the new line. Align the Plane with the edge of the thread as shown.

Go to Plan view. Draw a line into the model to act as a guide. Draw a 'Tangent Arc' using the line as the start point Drag in and down into the solid.

Pull the Surface with the 'Sweep' option using the 'Arc' as the 'Path' -  Full Pull.

I cannot get the bottom 45deg taper on the pin to work out

If you just want a 45° angle then do as I stated.

There are a number of ways you can finish the end i.e you could just draw a triangle to use as a cutter to cut the end to look like a 'chamfer'.

To do this Select the Axis for a new Sketch Plane. Draw a 45° Triangle at the bottom.  Pull this Surface to use as a 'Cutter -' Full Pull.

Hi Lauren, i really hope this arrives with you as i've had a hell of a time learning how to post reply's properly!

Right, lets just quickly say i think Jacant's last post is exactly what you want.

Sunday i made up the image below to help you understand but posting it wasn't possible until Jacant anwserd my appeal.

so, hope it's clear and helps with your undeerstanding.

In more than 2 decades of mechanical design and detailing i've always finished of machined threads of any sort as shown.

Threads on tapering screws that are self tapping ( to some extent) whether into wood ( normally)  or self cutting into metal ( but these are special with drill bits on the very end !) have the thread tapering into the screw as Jacant has shown or similar as Spaceclaim has demoed on youtube many years ago - but still up if interested :)

Enjoy.

I couldn't get it to ever cut the thread when I did the triangle method. I would amend the cylinder, but not the thread. It also wasn't letting me combine the thread and the cylinder. I did have the same conclusion as you both for modeling the threads though. I appreciate the amazing help and support from the community.

Lauren - Hi.

This is easy enough to fix as i think you just need to know about parts, components and what you can do with a surface depending upon what 'owns ' what  or is the 'Child' of another. Some playing with this will quickly help you learn.

So, to do the above simply, start a new file, on the sketch plane as presented, select the cylinder from insert tab, click start/end positions, enter / click to set diameter ( i know you know this but please keep with me). presented to you now is a sketch plane on the center line. Now draw a simple 'basic' triangle to represent the thread profile - when done, press 'D' key to display the solid view - now in structure browser you will see the triangle has been made into a surface the the cylinder is shown as a solid.

Select the surface and pull around an axis selecting a helix etc as / after you have pulled the surface, in structure browser the surface has turned into a another solid - now you have 2 solids only.

To 'Combine' the solids, hit 'I' or select Combine.

Select the primary part to be the most important to keep - thus keeping it's name that you might have chosen. move the curser off the part to change the mouse icon for next action. By default it changes to a saw ( to cut something away) - you don't want this so either select the Add bodies click icon or press Ctrl and select the thread.

Now thread and Body have combined and only one solid is in the structure tree.

Now with sketch cmd, on the axis draw a triangle in postion to chamfer where you want.

Now coming out of sketch into 'D' or 3D design view, there is now another Surface to pull cut. Select the surface , choose pull cut (minus sign) select the axis icon, select the actual axis, select 360 degs full rev option, and the chamfer is made on the previously  combined solid - cutting triangle disappears . if you want to keep the cutter after pull operation, you must copy it first try it, you'll see another surface show in browser after it's been pasted.

The Surface being pulled in this pull-cut operation, will only affect it's own siblings and i mean ALL of them providing they are displayed / visable not cutting hidden siblings. It will not cut another part that is owned by another component.

If you play - experiment with this all will become clearish gradually - it did for me!

If the surface does not cut perhaps ( in a more complicated design ) it has the wrong owner - then , drag the surface in structure browser to underneath the part owner ( either root or owning component you want to cut.

I think the problem was you had two separate solids not owned by a single parent or root and the cutting chamfer disappeared after the initial pull cut.

Cheers.

...... I couldn't get it to ever cut the thread when I did the triangle method. I would amend the cylinder, but not the thread. It also wasn't letting me combine the thread and the cylinder......

What have you got in the Structure tree?

Have you got separate 'Components' for the Thread and the Cylinder?

If you have then open one of the Components in the Structure tree. Grab the Solid and drag it to the other Component.  Now try to Combine. If that does not work then the Thread and the Cylinder are not touching enough to create the 'Combine/Join'

Select the inside face of the 'Thread' and 'Pull' it into the Cylinder. It should Combine/Join automatically. Or Pull the Cylinder diameter out slightly until they do merge. You can Pull the cylinder back to it's original diameter once they are joined.

The Triangle method above should work now.

Nice to see you here Tim

The Surface being pulled in this pull-cut operation, will only affect it's own siblings and i mean ALL of them providing they are displayed / visable not cutting hidden siblings. It will not cut another part that is owned by another component.

When doing a 'Cut' (-) it will affect other Components. An 'Add'(+) will not.

In the second Gif the Surface is not part of any Components. So a new solid is created.

In the third GIf the Surface and the solids are part of the Component. So all solids are joined as one.

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