How to stop a pipe rotating in 3d print
Are you OK with starting over from scratch - or are you looking for a "that's good enough" answer?
I see:
Move is almost always the wrong move as used by beginners.
Align that is not needed.
Offset Face(s) not needed.
Unconstrained sketches.
Fillets that could be in one feature.
Left over bits of geometry that do not appear aesthetically pleasing and I suspect are unintentional.
I also see asymmetrical geometry that I would expect to be symmetrical.
The deeper I did - the more issues I find.
Start a new file
Create a sketch of a 4-sided Polygon centered at the Origin on the XY Plane as shown below...
add the dimension shown...
now add a Vertical constraint between the two points shown.
What do you note about the color of the sketch after adding the Vertical Constraint?
Attach your progress file here (we will go very slow at first and then pick up speed as I see you are following along.
Next thing we are going to do is sketch a bunch of rectangles (one-at-a-time).
Start a New Sketch on the XZ Plane.
Sketch a 2-point Rectangle with the lower left corner at the Origin...
Right click on the Vertical line connected to the Origin and select Centerline...
You should see it change to a dashed centerline type.
Add the two dimensions shown below...
Note that when you select the Centerline that the dimension is a Ø35 diametral dimension.
Notice that if you hover over the first dimension that Fusion indicates the variable name for that dimension is d1
Extrude the first sketch by a distance of -d1
this insures that even if we change the original size, we will always have a cube.
Now Edit Sketch your second sketch (actually named Sketch3 in your file as you must have deleted Sketch2, that is OK).
Add a Horizontal line between the Midpoints of the two vertical lines...
Revolve the lower rectangular profile with the setting shown below.
Be sure, be sure, be sure to set the New Body option.
Click on the eyeball for the second sketch to make it visible again (if hidden) and repeat the Revolve New Body for the top rectangle...
Hide the visibility of the second sketch.
Click on the second sketch and select Edit Sketch (the solid geometry will temporarily disappear as we are going backwards in history to make a change).
Add the rectangle shown below...
Be sure to select the Centerline and then the corner to get the diametral dimension (I think you have this figured out now).
Hide the second body...
..
Revolve the second smaller rectangle with Join to the upper cylinder.
Now add a Thread feature to the smaller cylinder (do not checkmark Modeled yet).
Add a Chamfer to the edge of the thread for lead in ...
Now go back and right click on the Thread Feature and select Edit Feature and set to Modeled. Must be done in this order. We have another change to make to the thread to make it easier to 3D print, but we will come back to that step later.
Now hide the third body and select the Hole command and then select the top of the cylinder off-center as shown below and set the Options as shown....
Now click the Top view on the View Cube in upper right corner of the screen and then Click and Drag the center of the Hole feature to the center of the circle.
I always click off-center and then drag to center as I have seen too many instances of where user thinks they selected the center but are off by a tiny amount that is hard to diagnose the issue later.
Add a 1.5 Chamfer to the edge of the hole for lead-in.
You should anticipate the next step...
Edit the Hole feature and change the thread to Modeled.
Attach your progress here for next set of steps.
There is something fishy going on, but close to bedtime for me.
I'll figure it out tomorrow and let you know.
But if you have the time and motivation - start a new file and see if you can reproduce the odd behavior or if it works as expected on the second attempt.
Did you use the same thread parameters that I did M20x2.5
