Aligning a thread

[cnelhams]

I've created a thread on the internal wall of the lid and I need to match the thread on the external wall of the bottle. I've looked everywhere and can't find anywhere that explains this. Can someone please help, there must be a way of doing this in an assembly to make sure that the threads align properly. Thanks!

[StephenW]

There is no "right" way. I've used an insert and offset distance along with an angle offset to orient to get the thread lined up.

That being said, I've only modeled threads to use for 3D printing. I never model threads for production drawings, only cosmetic threads.

[John.Pryal]

I think if I was doing this I would start with the bottle (complete with thread) & then create an assembly of the bottle & lid in the closed position & make a 'component cut-out' leaving an impression of the thread in the lid. This way you could then offset the thread surfaces in the lid to create a little clearance between the parts & extent them to create a run-out. Hopefully this might assist you. Good luck.

Regards

John 

[cnelhams]

Thank you! This is how I thought to do it, just having a little difficulty making it work.

[cnelhams]

Hi John, 

I have finally got this to work, so thank you!! I'm planning on getting these components (the bottle and the lid) 3D printed for part of my university project. So my next question would be, once I have created the cut out on the lid, how can I save this component separately so that I can get it printed with the cut out section? Thanks in advance!

[John.Pryal]

I am not fully understanding what you are asking here. Is the lid not already a component (part) in its own right? I thought you had a bottle part & a lid part assembled together, then a component cut-out was made leaving the thread impression in your lid part. If you then opened your lid part only, the thread impression should be visible & shown in the model tree as 'Cut Out id .....'

Regards

John   

[kdirth]

Here is what I do when I need to create a matching surface:

• Assemble the parts in an assembly
• In the donor part, create a coordinate system to match the default coordinate system of the receiving part
• Save the donor part as an IGES using the matched coordinate system
• Import the IGES into the receiving part as surfaces
• Use the surfaces as needed

This prevents external references making the part independent of other parts.

An extra step to take, to limit the number of surfaces imported, would be to copy the needed surfaces in the donor part and select that quilt when exporting.

[TomD.inPDX]

I know you have your answer but I thought I'd add this for completeness since I seem to be doing this a lot for the very same purpose.

1st of all, the 3D print will want clearance built in around the thread.  Typically not much, but some.

The second issue comes with Creo in that it really doesn't like doing helical sweeps.

They often fail for various reasons.  You have to account for trajectory offsets that often work from opposite ends.

The only way I've learned to get around this, when it is critical, is to plan the helical sweep -carefully-.

What I mean by that is to do the math and match the sweeps at the appropriate time in each model.

Then, when you assemble the 2 parts, they match, even if you change your thread parameters.

Another method is how you deal with Boolean operations in Creo.  In the assembly, highlight the part you want to remove material from.  RMB-Activate.  Now under Get Data tab, you will find the Boolean operations that works directly with part models.  Neat stuff and works wonderfully if it doesn't error out.  You should be able to offset the thread surfaces and solidify those to make the clearance you will need.  ...or do the subtract function on the cap; make the STL of the cap, and change the master thread on the base to provide clearance.  you should also be able to make the subtraction model non-associative so things don't change blindly.

[TomD.inPDX]

I would remiss if I fail to mention a simple top-down engineering option.

Make a master sketch of your thread in an assembly model.  Know all your parameters and build them into an intelligent sketch.  Things like Z-offset, radial offsets, clearances and edge treatments.  Do the real work here.

Next, assemble the two parts that will make up the body and the lid into the assembly file with the thread master sketch.  Work on your top and bottom parts independent or by activating them inside the assembly.  When it comes time to cut the threads, use the master sketch to lock the positions and limited parameter of the threads.

These are external references in the words of Creo.  It is often frowned upon on the one hand but also highly praised on the other.  In your instance, it seems a perfect opportunity.  This is a paired set and this will keep it that way.  You will maintain 3 files in the design.  2 parts for 3D Printing export and an assembly file to drive the threads reliably with the ability to make easy adjustments if needed.  The real challenge is to avoid circular references.  Creo will help you there.  Use smart and limited reference selections from the assembly file while creating the part files.  Making changes will drive you crazy if you don't.  With some practice, this can drive an entire multilevel design.  There are optional software extensions that take this idea to the next level.

Please remember that helical threads are fussy in Creo.  Find an appropriate place in the model tree to cut the thread and continue your design elements.

[mbonka]

Clear and smooth method, with described possible problems...

Great answer...