Double Checking Your Work and Subverting Mr. Murphy

I once saw a graph that showed the cost of making a change in the CAD model vs  further down in the product design cycle

Spoiler alert! It gets more expensive as you move from design, to prototype, to production.  

One need only to cases like the Takata airbag recall, or Boeing 737 Max grounding or the impact of the impact of a a production level design change in in money, company reputation, and tragically, in lives lost. 

But I'm not here to write about such heavy topics. The example I'm choosing to document is a much lower stakes version of the same thing.  It's just a basic hobbyist example that at worst, is inconvenient and marginally embarrassing.

It's an access panel based on something you'd find on an aircraft. It's a concept for a potential future hobby project. I built one back when I was in school.

So I happily modeled away in Fusion 360, creating sheet metal parts and placing fasteners from McMaster Carr. 

After spending a couple of evenings of casual modeling, I was done! I took that moment we all love, I leaned back, looked at my work proudly, then prepared one last check before I took my little victory lap.

The completed inspection hangar, or so I thought...

And that's when I saw it. 

The countersunk rivets I had installed were the wrong ones. I'm not sure how I missed it initially, but obviously I did. 

So first, what's wrong with the rivet? 

It's a rivet with a 78 degree countersink, which means the countersink extends to the second sheet of metal being riveted.  This is a big no-no. When the countersink extends into the second piece of metal, the larger hole required in the first sheet of metal makes for a weaker joint.

The wrong rivet. I did match the countersink angle to match the rivet for clarification.

The incorrect rivet for this application. The countersink angle is too steep

The correct rivet is a 100 degree rivet. The shallower angle prevents the head from punching into the second sheet of metal. That means a stronger, and safer joint.

The 100 degree rivet, the correct one for this application. 
I know in the model the rivet does appear to just clip the second sheet.
But past experience has taught me that this combination does work.

The shallower angle of the 100 degre countersink makes a stronger joint

So that's the technical aspect of it, what's the other lesson?

I suppose the first lesson is make sure to check the hardware before you put it in. But we all make mistakes. That's where double checking comes in. 

A final check can help prevent the last little "oops" from slipping through. Even though we can't eliminate them all, we can reduce them with a little time. 

For those of us working in industry, a second set of eyes never hurts. In some places, multiple checks on a drawing are required. It's not a bad practice at all, one I think should be taken advantage of whenever possible. 

Some may argue it takes time, but it takes much less time than undoing a costly mistake. 

I've worked in maintenance shops where "second eyes" is a standard policy on items such as fuel system repairs. In other words, the person performing the work checks his work, and then a second technician or inspector checks it again. There often are even signatures required to prove that this step was performed. 

But that's it for today's anecdote. I re-learned a few lessons in a safe environment where the only bruise was to my pride. 

I hope you can take a few lessons from this musing, and keep making cool stuff! 

About the Author:

Jonathan Landeros is a degreed Mechanical Engineer and certified Aircraft Maintenance Techncian. He designs in Autodesk Inventor, Siemens NX, at work, and Autodesk Fusion 360 for home projects. 

For fun he cycles, snowboards, and turns wrenches on aircraft. 

Additional Resources: 

A nice  rundown on different types of rivets by- Hanson Rivet and Supply

A wealth of knowledge on general airframe repairs (start at page 4-31 for the Riveting Section) -Aviation Maintenance Technician Handbook 

Standard Parts Used on this Project.

.125 Diameter, 78 Degree Solid Rivet (The Wrong One) - McMaster Carr Part Number 97483A075

.125 Diameter, 100 Degree Solid Rivet (The Right One) - McMaster Carr Part Number 96685A170

10-32 Floating Nut Plate - McMaster Carr Part Number 90857A129

.094 Diameter Rivet (to Fasten Nut Plate) - McMaster Carr Part Number 96685A143

#10 Flat Washer - McMaster Carr Part Number 92141A011

10-32 Pan Head Phillips Screw - McMaster Carr Part Number 91772A826

Designing for O-Rings and Reusing Design Features in Fusion 360

O-ring seals are hard to avoid as a mechanical designer of any type. They can be found just about anywhere that fluid, gases, or debris needs to be kept in or out of something.

An O-Ring on the end of a flashlight

As simple as they appear, there's enormous amounts of research invested in that simple, pliable polymer ring.

How does this affect the designer? Typically by the pages and pages (real or virtual), containing tables and tables of o-ring groove dimensions.

O-Rings from a
different flashlight.

When it comes time to apply that to a 3D modeler, that means creating the o-ring grooves, including some tight tolerances. The process can be extremely tedious, especially when there are multiple o-rings of different sizes involved.

So how can a user create these o-ring glands as painlessly as possible? Sure, many of us have placed the same feature so many times we have the dimensions memorized. But why do that, unless you like that sort of pain? 

While I can't speak for every CAD tool, many tools have wizards that will help create o-ring glands, as well as other common design features. Autodesk Inventor has iFeatures, Solidworks has Library Features.

Fusion 360 doesn't have a library feature as such, at least that I've found at this point. But, there is a way to create such a thing and make life a little easier.

Preparing the O-Ring Gland

The first step, is acquire the documentation with the necessary dimensions. Lately I've become partial to the Parker O-Ring Handbook myself, seeing how they know a thing or two about sealing. 

For this example, I'll use a -018 o-ring. It's a static (non moving) seal, and I'll use the male gland as an example (stop snickering, that's Parker's terminology). 

Gland Schematic from Parker O-Ring Handbook

Here are the dimensions pulled from the design tables

From Table 4-1

C=.860/.861

F = .750/.754

Corner break = .005 

From Table 4-1A 

W = .105/.110 

From Table 4-2

R = .005/.015 

O-Ring Groove Radius

Modeling the O-Ring Gland

Before creating any models in Fusion 360, enter the relevant values into the parameters dialog box. This seems like extra work, but I think it makes creating models with new sizes easier.

The Fusion 360 Parameters screen with the o-ring parameters started

Now, draw the profile of the o-ring gland, using the values from the parameters table. 

The gland profile sketched and dimensioned.

Next revolve the profile into a solid. Now, we have a solid representing the shape of the groove.

The o-ring groove revolved as a solid.

Believe or not, that's it for creating the gland. Saving it will make it available for other components to use.

Inserting the O-Ring Gland

What's needed next is a component in need of an o-ring. In this case, I've modeled a simple plug in Fusion 360.  It's similar to the threaded plugs found here on the McMaster Carr site.  I've just moved the gland location to make things a little more clear.

A threaded plug

To place the o-ring gland, right click on the file in the Data Panel and choose "Insert into Current Design".  This places the gland into the model

This inserts the gland into the plug.  Now it can be positioned by using the Move/Copy command, or assembled using the Joints command.

Placing the o-ring gland. The Move\Copy command is shown.

After positioning the gland, use the combine command to subtract the gland volume from the plug.  

Once the Combine Command has been committed, the plug is finished.  And you also have a -018 gland ready to use in your next design!

The finished plug. (Don't forget to hide the original solid!)

But undoubtedly, other o-ring sizes will be needed.  That's where using the parameters can come in handy.  Just copy the existing gland and rename it, then enter new values in the chart.

Summing it Up

I only used static o-ring grooves for this post.  There's also dynamic (moving) seals, face seals, glands that use backup rings (for higher pressures), and probably something else I'm not mentioning. I just can't get into them all, but the data is out there. It's just a matter of looking and asking questions.

As for desigining the gland, the steps I've shown here are for Fusion 360. But if you've made it this far, I hope it's the process you take away. I hope that you can find it helpful, and perhaps can apply it to what ever product you use for your design.

At the very least, I hope you walk away with resources that you can use when the time comes to design for o-rings.

And lastly, here's the list of resources I used in this post.

Parker O-Ring Handbook -  PDF Download

McMaster Carr - Website

Milwaukee Penlight - From the Home Depot Website 

Mag Instruments Maglite - Mag Instruments Website

Autodesk Fusion 360 - Autodesk Website

Lessons from the Shop Floor - Helical Inserts do more than Repairs.

Many technicians, designers, and fabricators are familiar with helical inserts, often referred to by their trade name "Heli-Coil". 

A helical insert in an exhaust manifold

These inserts are made of a coil of diamond shaped wire. Looking like tightly wound spring, they can be installed in a special threaded hole to create standard metric and imperial threads.

In my early experience, I only saw them used to repair a damaged thread. As a matter of fact, they were used for thread repair so often, the name "Heli-Coil" became a verb. 

"Curses! This thread is completely boogered up! I'm going to have to Heli-Coil it! This why you always start a screw with your fingers!"

But as I gained more experience, I saw two additional uses for helical insert, and that's what I thought I'd share in this post. 

Wear Resistance

A 3D model of a free running (non-lockng) 
helical insert in an aluminum block

The first is to create a wear resistant hole in softer material, such as aluminum. Instead of waiting for the hole to get worn out, a helical insert is installed in the hole at the time of fabrication. The helical insert is made of a more wear resistant material such as stainless steel, although there are other materials available. This creates a more durable hole better suited if repeated installation and removal of the fastener is expected.

You might see this on a panel that needs to be removed periodically for inspection. Naturally, once the inspection is competed, the panel needs to be reinstalled. The more wear resistant helical insert lasts longer, and resists damage caused by cross threading. 

And if you have a really bad day and damage the insert, it's possible to remove the insert and install a new one without damaging the base material. 

Create a Locking Element

A 3D model of a locking helical insert.
Note the deformed thread in the middle.

Another element is to create a hole with a locking element in it. Locking helical inserts have a distorted thread in the middle that resists the screw backing out. By using a locking insert, the need for a screw with its own locking element, such as a nylon pellet, can be eliminated.

While this may seem like extra work for not much gain, this can be advantageous since you don't need to purchase fasteners with their own locking elements. Another advantage is in higher temperature applications where a nylon locking insert's performance may degrade to the point where it loses effectiveness.

And just like it's non-locking (also known as "free running") counterpart, it can be removed and replaced ,when it's locking element loses effectiveness.

 Wrapping it up

I've written this post based on helical inserts, but there are many styles of threaded inserts. Far more than I know about, let alone discuss in one post. So if the helical insert isn't your speed, there's likely another that will do the trick.  

For a sampling of just some of the different types of threaded inserts available for different applications and materials, take a look at the McMaster Carr catalog!

I hope you found this post helpful and informative. 

Let's get out there and design, fabricate, and maintain some stuff!

Appendix and Credits

• 3D models created in Autodesk Fusion 360.
• Threaded insert models downloaded from McMaster Carr
• Threaded insert models are based on the NASM/MS21208 standard for non-locking inserts, locking inserts are based on the NASM/MS21209 standard, although several standards, both imperial and metric, exist.

Finally! Looking for a video on how to install a helical insert? Check out this video here! 

Photo Credit: rustyheaps Repairing exhaust manifold, XK engine via photopin (license)

A Challenging Channel - Modeling a Sheet Metal Channel in Fusion 360

On a morning this weekend, while hanging out at home with my coffee in my hand, I decided to play with Fusion 360.  I had a part picked out that looked simple enough.

The finished part. It looks simple, but it hides a suprise

The part I chose looked to be a simple sheet metal part.  It looked to be a simple enough part, but it did have a joggle in it that complicates things a bit.

The joggle that changed how this part was made

Since it's got this joggle, it can't be easily modeled using sheet metal tools.

The sheet metal version wasn't quite what I was after.

So I decided to model it using the "regular" modeling tools.

I also decided I'd document how I did it here, for both posterity's sake, and in the hopes that it might give another struggling user an idea.  I won't go through every single step, but I will give an overview that hopefully encompasses the high points.

The first thing I did was model the envelope.  I nothing more than an extruded rectangle.  A "brick".

The starting point. An extruded rectangle representing the parts outer dimensions.

Next came the process of carving out the shape. I started with the joggle.

The joggles cut into the part. I've turned one of the sketches on to make it more visible.

Once the joggle was in, it was a matter of adding the remaining features, including the outside fillets that represent the outer bend radius.  Notice that the part is still a brick.  It's just a brick with some nice looking features!

The brick has all the features of the sheet metal part now.

This is where my original plan went wrong. My plan was to use the shell command to create the inner profile.

But for some reason, I couldn't select the surfaces I wanted.  I always ended up selecting a surface I didn't want.

So it was time for plan "B".  I switched to the surfacing workbench and used delete face to remove all the faces except those that represented the outer profile of the part.

The part with all but the outer profile removed.  

Now that I had only this surface, I was able to return to the solid workbench and use the thicken tool to get the final shape I needed.

In Conclusion

So is this the only way to do it?  I doubt it.  But it did get the result I was after in a way I was happy with. I'm sure someone out there has a different way of doing it, they may prefer it.  And maybe someone out there has a way that's truly better.  I would be thrilled if they do and I hope they share it!

How would this part be made in real life? 

This is one place that I'm not an absolute expert, so I encourage others to chime in.  But I do have some experience making sheet metal this way.

In production, a blank would be placed in a die, possibly using two of the holes to locate the part.  Then a press would push the two die halves together, forming the part in one operation.

Here's a pretty good video on this process used for the ribs on an aircraft wing.

If the part is made in low production, A form block can be used, made out of wood or metal.  The blank is then formed using a hammer.

He's a video on that process. While this video shows the process being done for steel, aluminum would be done in a similar manner.

The part I modeled in Fusion 360 calls for 24ST aluminum, which is the equivalent of 2024-T3. I know that 2024-T3 can crack when formed around tight bends, so it's possible they would have used 2024-0 (dead soft) and heat treated to the -T3 condition afterward.  But that's one place I'd have to defer to the sheet metal experts, feel free to chime in!

And that's it, I hope this video was informative!

A Final Addendum, Murphy's Law Strikes! 

As I finished up this post, I tried the shell one more time.  Guess what! It worked! It seems I was just not quite getting the picks and clicks right when I tried it earlier.  But I decided to go ahead and share the post anyway because I still feel it's a viable alternative. 

It figures! The shell does work!

A Brief Summary of Drafting, Modeling, and Making Hydraulic Ports

Somewhere, someone is saying "It fit when I modeled it in the compuuter!"

CAD systems are wonderful tools, but, they're still tools, and largely reliant on the person pushing the mouse.

I was reminded of this when talking to a colleague about the standard hydraulic ports we use.

I know, riveting, right?

The conversation eventually turned to how the ports are called out on the drawing, and how we didn't learn this part of it in engineering school.

I recalled a time when I didn't know the standard, and how mysterious the process seemed to me as a young engineer

But when I was just a young lad, there was a crusty old salt with a black substance on his fingertips.

I'm not sure if it was grease, ink, or pencil lead. It may have been a combination of all of it.  Regardless, he helped set me straight.

So I decided I'd share what I know about the design, modeling, and drafting of hydraulic ports, in the hope that maybe it'll help someone else who faces a similar challenge..

The ports in question are "straight thread o-ring ports". In short, it's a port that allows an o-ring to be squeezed between the port wall, and the hydraulic fitting. This is shown in the image below.

The o-ring is compressed between the fitting and the wall of the port, making for a good seal.

It would stand to reason that the geometry to create the seal is pretty specific, and you'd be right.  That's where the standards come into  play. Somewhere, in the past, someone put a lot of work into figuring this out!

The one I use most at work is the AS5202 standard, it's the one shown in this image above. There's a lot of little details in there, fairly tight tolerance dimensions, angles, and surface finishes.

I won't go into all the dimensional details here, but for reference on the different port sizes and dimensions, the Parker Hannifin document can be referenced here. Rumor has it they know a thing or two about fluid fittings! The AS5202 port data can e found at the top of the document.

So, given that these dimensions are standardized, how do you make these ports?

I'm not a leading authority on the subject, but I know of two ways to make these ports.

The first, is get one of those fancy CNC machines and do some programming.

The other, is to get a tool that already has the port profile cut into it.  Then all you need is a standard mill.  You might even be able to use a drill press, but I'd defer to a real machinist on that one!

The threads are added in a secondary operation.

An example of the tools can be found at the Scientific Cutting Tools catalog page here.

AS5202 Port Tool. Image from Scientific Cutting Tools Catalog above

If you'd like to take a detour and see a machinist using a similar tool to make this port, you can check out the YouTube video here.

So now there's a discussion on the port, and how it's made.

But, how would you call these out on a drawing? While I'm sure everyone has their own method, one thing that could be taken away from this is to.... .use the standard.

Just callout the port: "by the standard"!

An example of a typical port callout

That covers some of the "big stuff", but here's a couple of trivia notes for you.

The dash means someting!

If you look at that document, you'll notice the column "tube dash number". That's a standard that seems to be one of those that the initiated assume that everyone knows. 

Notice in the image below, taken from the Parker Hannifin catalog.  You'll notice there's a column for "Equivalent Dash Nmmber", as well as a column for "Tube OD Minimum".

Now, if one takes the dash number, and divides it by the number "16", you'll end up with the Tube OD.  It's like they did it on purpose!

So if you're using -4 tubing (.250 inches), any fitting using a -04 dash number will work.

\

An example of a fittings and tubes

The standards change, but the geometry doesn't.

You might have notice that there are three standards that are listed as "Superseded" in the Parker Hannifin catalog.  And that's because the standards have changed over the decades, but the actual geometry has changed little, if any.

Some of you may even know it by the older designations!

I guess they had the geometry right even then!

The "Supersedes" comment gives you a brief history of the port.

In Closing....

I hope this little blurb was helpful. While it may be mundane and boring to some, I actually think it's interesting.  So take a look, see if it, or some form of the information helps you out.

Happy designing!

Which CAD System is the Best? Guess What? It Depends.!

FIrst the Earth cooled, then I started my 3D modeling career with Mechanical Desktop....

A picture of my first engineering meeting.

Eventually I'd crawl out of the 3D primordial ooze and move on to Autodesk Inventor. That would be my tool of choice for much of my career.

A coffee table I modeled in Autodesk Inventor a few years ago

Lately, the shifting sands of my career have led me to use Fusion 360 more heavily for personal projects, and Siemens NX at work. I've even had an opportuntiy to dabble in Solidworks a bit, although I've only become acquainted with it.  

I'm far from an expert in every tool, I'm still far more capable in the Autodesk tools than I am in the Parasolid based tools such as Solidworks and Siemens NX.  

But I'm not writing this to claim "this CAD is better than that CAD". In fact, I'm going to avoid making statements to that effect.

There are plenty of bars, pubs, and lunchrooms where that discussion can be held! 

What I am going to do, is share what I've learned having been exposed to all these different systems. If you take a few moments out of your day, I leave you to draw your own conclusions.  I would even be as bold to say that there are some who have already made their conclusions. If that's the case, I doubt I could say something to sway you, if that were my intent.  

To that group of users, I say "Rock on, get down with whatever CaD system you've selected.

So here you are, a few things I've learned interacting with a few different 3D modeling tools.


1) They're exactly the same, except where they're different. 

I've learned that in general, most CAD programs can get your job done, especially for most common functions. The biggest difference is how they get there. Do you want to place sketch constraints in Inventor, there's a tool, and a workflow for that.  Do you want to get the same result with Fusion 360, Siemens NX, Solidworks, there's almost certainly a way to do it.  

A B-17 Bombardier's panel I modeled in Fusion 360

Certainly a case can be made that one workflow is better than another. I'm sure some of that is a matter of personal preference, and in others I'm sure that a workflow in a given program can indeed be better.  

2) The next tool isn't just like your old tool, get over it. 

Change can be hard. I get it! And I'm no better than anyone else when change comes, stands at my cubicle and says "If you could change everything your comfortable with, that'd be great."

A bracket I modeled in Solidworks. It's certainly different than Inventor, but similar to Siemens NX

I'm currently in the process of learning Siemens NX after using Inventor for 20 years. NX is a great tool more than capable of doing the job, but there are a few places where Inventor runs circles around NX in ease of use.  

Sure, I could jump on my desk and scream "You can have my Inventor when you pry it from my cold, dead hand!" But ultimately, the company, you know those guys who write my checks, have decided NX is the way to go. It's up to me to be part of the team, or be that one worker that's so toxic that my comrades take the long way to avoid making eye contact.

3) Learning a new program can be a great opportunity to "skill stack".  (I said "skill stack"! Buzzword achivement unlocked!)

While embracing a new product can be a frustrating challenge at times, I chose to see it as a chance to expand my skills.  And I've found that by approaching a new system with an open mind, learning a new system isn't as daunting as it might seem.  Many times, tools are similar enough to one and other where I already know a big portion of a workflow. 

I've sat down with Solidworks and tried something and realized, "That's similar to NX!" They both use the Parasolid kernal after all. 

Likewise, I've that other tools have similar workflows to each other, and once you know one, it's not as hard to learn the next. 

I can now sit down with someone and say, "I've used 6 different CAD systems, and administered two of them".  

Am I an expert at all of these systems? Absolutely not. But I have the ability to pivot into a new tool and learn it if I need to. And 3D modeling isn't my only trick, I have my engineering and design background to fall back on. 


4) The best CAD system is the one your getting paid to use.

We all have our favorite CAD systems, that we'd use if we were independently wealthy, and could run whatever we want. But most of us have to use the program dictated by the company we work for. 

Is that a bad thing? I think that's for everyone to decide for themselves. I've learned (the hard way sometimes), to do by best to be passionate about the program paying my bills, even if it might not be my first choice of programs.

In conclusion, these are just my ideas. If you disagree, that's completely fine!  This is me on my little soapbox, waxing poetic about the way my career has been shaped.  

I encourage you to reflect on your own career and where it's taken you, and live that potential to the fullest. 

Acknowledgements:

photo credit: trustypics - Swiss Army Knife

photo credit: LadyDragonflyCC - Wrenches

Speeding up a 3D Print with Chamfers

A section view of a hollow part that will need
a lot of supports to print  successfully
Model created in Fusion 360

When I first started 3D printing, I had quite a few assumptions  in my head.  One of the first assumptions I had to dispel was that if the model was finished in CAD, it was ready to print.  There was no such thing as optimizing for 3D printing.

I was quickly learned that like many projects, preparation can be a huge part of making sure a you can get a print in a timely matter, and optimizing for 3D printing was a very real consideration indeed.

One of the things I've found I modify a lot are the hollow internals of the part.  That's right.  Sometimes the portion of the print nobody ever sees gets the most attention!

If you're like me, you might think "Who cares what the inside looks like?  Nobody sees it."

The rub comes when considering 3D printed models need to build a lattice work of supports to hold up overhands that would otherwise collapse if left unsupported.  That lattice work takes time and material to create. 

The supports (generated in Cura), can be seen in cyan below.

The required supports for this build.  That's a lot!

And what that translates into, is a lot of extra time and wasted material as tons of supports get generated.

So what can you do to reduce the internal supports for  model?

Build your own!

At least in my experience, I found that the threshold where the slicer adds supports is 45 degrees.  If an overhang is 45 degrees or more, it will "self support".  So by adding 45 degree chamfers into the hidden overhangs of a model, the amount of time, and material needed to print a model can drop way down.

In this example, 45 degree chamfers removes the need for supports
(Image from Cura)

In the prints I've made, I've shaved about 30% off the time to print a model.  In one case, I saved 10 hours from a multi-day print.

Of course your results will vary, but the real lesson I'd like to share is that sometimes, you may find that it's better to make modifications to your model in your preferred CAD system before throwing it at your slicer and letting that go to town.

So think about altering the internals of your models a little to remove unnecessary material.  Something as simple as adding big chamfers to overhangs can make an enormous difference in your print times and material costs!

3D Printing Threads - A Few Tricks I Picked Up

When I first took on 3D printing, the subject of threaded fasteners always made me a bit nervous.  While I try to use actual hardware whenever possible, there are cases where the thread isn't used on a simple part that can be purchased from McMaster-Carr.

An example of a part requiring a thread

That meant, eventually, I was going to be faced with making a thread. What made me nervous was how to I make the thread work? Especially since I typically deal in machine threads? Machine threads can get pretty fine. 

First, I want to get the acknowledgements out of the way. I didn't come up with these ideas on my own.  I started by watching the following videos, and adapted them to fit my needs.  

The first is from KETIV Technologies, and the second, from 3D Printing Nerd.  Those videos are certainly worth taking a look. But I did need to tweak their procedure to get the result I needed.

So here's a quick rundown of the procedure I used, with a couple of changes I made to make it work for me.  

I'll be using Fusion 360 for this example.  I've found it gives me the best results, but I'm sure other CAD tools can perform similar functions.

 

Here we go! 

Thread Reliefs are Not a Relief

First of all the part I work with often have thread reliefs modeled in. I found out the hard way that these can sometimes interfere with the thread lead in.  I've had the best luck deleting them and making sure the thread starts right at the end of the desired starting point. 

The thread relief has been deleted.
Click image to enlarge

Tune up the Virtual Tap and Die Set

After deleting the reliefs, the modeled thread needs to be added.  This may be done by editing an existing thread, or creating a new one if a thread feature doesn't exist. Fusion 360 has a check box that models the thread,  Other programs have different methods of adding the thread. 

The modeled thread and dialog box.
Click to enlarge image.

Practice Your Scales

Now comes my challenge and the solution I found for that challenge. I needed to scale the thread to increase the clearance between the mating thread so it will thread smoothly. But I can't scale the entire part, because the rest of the geometry needs remain the same size.  

So I split the part into two different solids.  In this case, I used an extruded surface as my splitting surface.  The diameter of the surface is only slightly smaller than the minor diameter of the thread.  

Remember the goal is to scale the thread, not anything else! 

An example of the surface that becomes the cutting tool.
Click image to enlarge

Now the solid containing the thread can be scaled. For the parts I work with, I only scale radially.  The thickness is left alone. 

Scaling the solid that contains the thread.
Note the use of Non-Uniform Threading
Click image to enlarge

As far as the amount to scale, I've found that it varies.  I've done between 0.5 and about 5 percent.  With larger percentages working for smaller threads. However, I'm still working on the guidelines, so I wouldn't consider these numbers absolutes.  

Check the Thread Clearance

As a final check, I compare the part to it's mating thread, assuming I have it, and if I have what looks like a good clearance, I roll with it. 

Comparing the mating threads to eyeball the clearance.
Click image to enlarge

I know it's not very scientific, but so far, it's been effective. 

Glue it all Together with the Combine Command

For my final step, I combine the solids back into one.  Now the part is ready to be exported as an STL file, and imported into your slicer. 

Combining the two solids back into one.
Click image to enlarge

Speaking of slicers, I use Simplify3D at work. And what I've also found works best is to remove any supports that are automatically generated inside the thread. I've found they aren't needed, it's just that Simplify3D thinks they are.  

And thus far, these guidelines have worked well for me.  Feel free to take them and give them a try, and modify them as you see fit!

Good luck! I hope this is helpful! I hope you can take these ideas and use them as seeds to develop your own. 

And please share your tricks with others! 

Jonathan (Jon) Landeros