Simple Thread Feature On Assembly Drawing

[HaroldRC]

The simple external thread feature used in part files and assembly model files is not displayed in an assembly drawing.  If the drawing is shaded, the threads are barely visible, but in a simple line drawing they do not appear.  The parts appear as smooth cylinders.  Checking the box in the Display Options window for Thread Feature does nothing.  How can I get a thread feature to appear on a non-shaded assembly drawing without spending a lot of time drawing a simplified thread image manually on every part in the assembly?

[gcoombridge]

@HaroldRC it is working for me in 2021.2.1.. 

Check the layer visibility for thread lines under standards library - object defaults (mine is on Hidden Narrow(Default)) 

[hosford]

Make sure this check box is checked, the threads will show up on a shaded view with out being checked, but is only an image.

[johnsonshiue]

Hi! Are you looking for physical thread, the actual thread geometry? Inventor treats standard thread as a texture for performance purpose, since the actual thread geometry may add unnecessary complexity to the design.

To create physical thread, you may want to install the following app. Please note that the threadModeler only supports up to Inventor 2020 officially. There is a way to make it work for 2021 (see the comments area).

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=2540506896683021779&appLang=en&os=Win64

Many thanks!

[HaroldRC]

The first image is the drawing and the second is the model.  I checked the styles editor and it was set on Hidden Narrow.  I tried a few others to see if it made a difference and it did not.  Producing hidden lines only shows holes in the part, but not the hidden thread lines.  The check box in the display options is checked.  The thread image in a shaded view on a drawing is too blurry when it is printed out, especially with large parts that have a fine thread.  I just want it to be easier for the guys in the assembly dept. to be able to see it clearly.  I can fake it by tracing a spline over the end of the parts and making a linear pattern, but that has to be done separately on each part and it is not worth the time.  Also, I tried a hatch, but it didn't look too good.  It would be nice to have a simple line feature similar to what it shows in the shaded view, but with fines lines so that they don't blur together.

[mcgyvr]

Thread representations do not show in non-shaded isometric views in Inventor..

I've forgotten if thats an Inventor limitation or how the drafting standards intend it to work..

[HaroldRC]

OK, thanks.  At least I know I wasn't missing something.

[johnsonshiue]

Hi! I believe this is per drafting standard. The actual thread geometry is too complicated and it does not add any more design information than the callout. Imagine an assembly with thousands of nuts, bolts, and threaded holes. The amount of compute power to represent the physical thread would be huge for no gain. This is why Inventor represents the thread cosmetically in 3D model.

To create the actual thread, it is actually a very interesting topic. The correct geometry needs to be modeled using Solid Sweep, because it is how the thread is cut. Profile Sweep or Coil can get it close but not 100% precise. For printing purpose, it is probably acceptable using Profile Sweep or Coil.

Many thanks!

[gcoombridge]

to add to what @johnsonshiue said - at the scale of many threads on a drawing page the thread helix with the root fillets etc... will appear solid black because of the density of the lines

[HaroldRC]

Ok, I think I have a compromise.  I created a surface coil.  On the sketch, I made a line on the surface.  The length of the line is the width of the crest of the thread.  This is easy to calculate as 1/8 of the desired thread pitch dimension.  I made the coil using the desired thread pitch.  In the model, this is in addition to and on top of the simple thread feature.

In the drawing isometric view, with the Drawing View window open, go to Recovery Options and check the box that says "Include Surface Bodies".  The fake thread coil will appear.

In a planar view, do not check the box to include surface bodies and you will have the standard hidden line threads because in the model, the coil is another feature added on top of the simple thread feature.

Adding the surface coil increased the size of the file, but not a significant amount.  A coil with 259 revolutions added about 500 KB to a drawing file.  Most of the time, you won't need 259 revolutions and it adds just enough detail to appear as a thread, but not so much that it appears as a solid black object unless you make it really small.  The thread in the image is 1/2-28 UNEF.  Also, you can change the pitch just for the appearance without affecting the dimensioning of the simple thread tool in the planar view.

[dan_inv09]

"simplified thread image"

So I think just

would be acceptable, except not just in orthographic views

sort of like

[dan_inv09]

That seems like a lot of work as well.

I just want to know why they can't do the simplified representation in isometric views. That's all I would need.

(Do I need to dig out the old drafting textbook if they throw back "It's per standard"?)

[HaroldRC]

Yeah, I'm a little obsessive and I refuse to take any medication.  If it was a single part drawing for only a machinist, then the standard ANSI representation would be plenty good enough.  However, on a busy assembly drawing for production people who don't like to handle drawings any bigger than 11 x 17, the threaded parts that appear to be smooth are going to be confusing.  At that scale, even the ANSI representation won't be discernable.  The people in production are not dummies, but since they are in a completely different state I cannot just walk over and explain it.  Also, it really is easy to do it the new way with a surface coil.  All you have to do is create a new sketch in the model file on a central plane and make one tiny little line at the surface.  Then just make a coil from that sketch and you're done.  You can turn it on or off in the drawing with a couple of clicks.  It's a personal preference, but it's still nice to have options.

[gcoombridge]

There's an idea created for it: Draw real thread in isometric views (without shading) - Autodesk Community

My approach is typically to shade the iso views and have the orthographics unshaded but I guess thats a preference thing. I the surface coil looks like a lot of work. You could also split the face at the thread run-out to identify the face...

[JamesSZHL62]

I have to turn this on in all of my assemblies. Is there a setting to keep them on so I don't have to turn them on when creating my assemblies?

[HaroldRC]

The only way I know is view specific. However, you can use the recovery option setting when you are placing the view into a new drawing. When you want to place a new view into the drawing, the drawing view window automatically opens. Just click on the Recovery Options tab at the top of the drawing view window and then you can check the box for Include Surface Bodies. You can do this when you are setting the scale and view labels, so you do not have to go back to the drawing view window after you have placed the view unless you are revising an existing drawing view.
Also, a tip for setting up the surface coil on the part in the ipt file. You don't need to do any calculation for the crest of the thread unless you are drawing a large thread like an ACME thread. For simple screw threads, the default line weight will display the thread coil the same as long as the coil thickness is less than the default line weight.

[johnsonshiue · Accepted solution]

Hi @JamesSZHL62 and @HaroldRC,

Some of the base view options persist on a last used basis (stored in the registry).

Launch Regedit.exe and go to the following folder (for 2025)

Computer\HKEY_CURRENT_USER\SOFTWARE\Autodesk\Inventor\RegistryVersion29.0\Applets\DrawingLayout\Preferences\DrawingFormat

Find "BaseViewDefIAM", "BaseViewDefIPT", "BaseViewDefIPN." These keys store the last used values of certain view options. "Thread" is indeed one of them. The quickest way to persist the option is to create a drawing view based on the desirable options. Please note that the options are also per source file basis (IPT, IAM, and IPN).

Many thanks!

[JamesSZHL62]

Thank you.

[JamesSZHL62]

Thanks!