Outer threads

hello, I just started using Solidworks 2004 about 2 days ago, so go
easy on me.
I'm trying to create a threaded rod, with the threads on the outside
of it.
that's about it, I have no clue what to do. I looked in the "hole
wizard" and in the toolbox, and didn't see anything
thanks
-Nick

 

Create the feature using the major diameter. Select the edge of the
feature. Select 'Insert...Annotation.....Cosmetic Thread'.

Jim S.

 

Jim's reply may or may not have answered your question, however what he did
answer is generally the proper thing to do. For the most part, you don't
model the actual helical threads on hardware because of the computer time to
handle them.

If you really need (or want) them, you need to do a helical cut. Start by
making the solid rod, create a helix, and sweep a cut along it. Or the
other way is to make the root diameter and apply the thread the same way,
only instead of a cut you would use a boss. Come back with more qestions -
this is a great place to learn.

WT

 

Nick, Here are three ways.

Method 1 - In the drawing as a cosmetic thread.
Easiest way is an Annotation in the Drawing.

Select the major diameter circular profile in the drawing.

Select Insert, Annotations, Cosmetic Thread or select Cosmetric
Thread from the Annotations toolbar. If you have the CommandManager
displayed you have to toggle between Annotations, Drawings and Sketch
toolbars in the Control Area (leftside) of the CommandManager.

To display toolbars, right-click in the gray area next to Help in the
Main menu and check the Annoations toolbar.

Enter the minor diameter, Select Blind (probably), Thru All (for
holes) or Uptonext (requires a face)


Method 2 from the Hole wizard - cosmetic thread option only works if
you have a hole. Not your current example - but this is handy when
you have interior holes. Lot less time and looks good for a picture
file.


Method 3 - If you really need the thread feature, example a plastic
bottle, you have to create a Sweep feature.

The Sweeep feature uses 2 sketches, path and profile. The path is a
helical curve and the profile would be the thread cross section. This
takes the most time and it should only be used when you really nead
the thread as a feature and not an annotation.


Here is a simple example:

Create a cylinder on the front plane as an extruded base feature.

For the path,

Select the front face of the cylinder and select sketch to open a new
sketch.

Click Convert Entities from the Sketch tools toolbar.

Select Insert Curve/Helix from the Main menu.

Enter pitch and number of threads.

Key point - Select the start angle at 90 (for cross section sketch on
the right plane). Click OK to exit the Helix.

Save and exit sketch1, green check mark.

For the second sketch, profile,

Click the right plane and open a new sketch

The simpliest thread profile to illustrate a sweep is circular, but
usually they have a tooth shape.

Display an Isometric view so you can see your helix and the sketch on
the right plane.

Sketch a circle on the right plane, above the helix.

A Sweep requires a Pierce relationship.

Select Add relations from the Sketch toolbar. Select the center point
of the circle and select the helical curve. Select Pierce.

Save and exit the sketch, this is sketch2.

You now have 2 sketches in the FeatureManager. The small circle is
attached to the helix.

Select Sweep from the Features toolbar, select Sketch1 for the
profile, select Sketch2 for the path.


You should also create a threadplane offset from the start of the
thread so you can adjust the starting depth - but that is another
lesson.

Regards, Marie

 

wow, thanks all of you, I REALLY need the actual thread.
I'm starting a business for RC Car after market parts, and am making a
gear adapter to be CNC cut, so i guess cosmetic's are out of the
question
here's some of the stuff i've made so far:
http://www.dualbl.com/sldwrks
thanks
-Nick

 

Hi Nick,

How long have you been using SW's?

Thanks,
Dan

 

Nick,

If you really want the sweep feature for the thread go through the
candle stick tutorial online. This example utilizes a an arc for the
path - use the helix. The xsection profile is an ellipse. Create the
profile of your thread. I'm not certain of the thread profile but it
probably is a V-shape or trapezoid shape.

Add a thread plane - on a motor shaft the helix can't hit the shoulder
because it can't be machined that way - so go at least 1.5 to 2 turns
from the shoulder to start the path.

Make the profile bigger that what it actual will be because it will be
easier to see when you pierce. After you pierce, then modify the
dimensions.

Utilize as many relations in the profile as you can - build in
symmetry.

When you pierce, the sketch has to be at the start of the helix - or
else this will not sweep. Sometimes when you pierce, the sketch jumps
to the middle of the helix. It is better if you sketch the profile
near the path closest to the side of the starting point.

Again - my first preference is a cosmetic thread - but when it has to
look like the the actual part then you have to do a sweep feature.



Regards, Marie

 

And remember, the sweep can be either a cut or boss - you decide based on
what diameter you start with.

WT

 

ok, thanks ALOT guys!
hopefully I'll be able to start making the parts within a week, and
i'll post pics when it's done.
I've been using Solidworks for about 2 weeks, and Solidworks2004 for
about 4 days now.
thanks
-Nick

 

And girl.

WT

 

hehe, sry, girls too
-Nick