How to stop a pipe rotating in 3d print
Edit - removed, my instructions, figured out a better way.
Back in a minute.
OK, I'm back.
Edit Sketch2 and add this rectangle shown in blue.
Oops, got called away again.
Now add these dimensions.
For the 125 and the 160 (to Origin) be sure to select the endpoints and NOT the centerlines.
Revolve the inner portion of the profile with Body3 visible and be sure to Join,
Make the sketch Visible again if hidden and this time Revolve the outer portion of the rectangle with NEW BODY.
Challenge 1.
Add the tapped Hole and the threaded rod to these components just like did before.
Challenge 2.
If the first challenge went OK, then add this cap at the end using same techniques (but don't do the Fillet, I want to show you a different way).
Very nice! You even made the hole drill depth a bit deeper than the thread depth - that is a pro move on your end. Not so important for 3D printing but critically important for mass production.
One thing to notice.
no red Lock symbol on your Sketch2 and a white dot in Sketch2. This means the sketch is not fully defined. White dots and blue lines should keep you awake at night. Click and drag that white dot. You will see that you have an extra line there. In this case you can delete it. In other cases you would add a Coincident Constraint to the endpoints to fully define location.
I will have more steps for you tomorrow. Getting close to bedtime for me.
Add your desired Fillet to the top post.
Then for the cap on the side post try the Full Round Fillet.
select the cylindrical face and then OK.
Observe the results. You don't have to enter a radius and if you change the cylinder the fillet will automatically update.
But if you don't want full round, then undo and add a regular edge fillet of desired radius - I just wanted to show you this fillet type.
Hide all but the first body.
Select Fillet (make sure not on Full Round Fillet) and then window select the entire cube body.
Enter the 5mm radius.
Now let's add the Hole to the cube.
Select the face of the cube away from the center.
Click and drag the center of the hole.
You should see a faint white dot indicating the center of the face.
Drag and drop the hole onto that Point.
Now Edit Sketch2.
Add the Vertical Construction line down from the Origin.
Add a Horizontal line is space as shown...
We don't like white endpoints and blue lines.
Add a Coincident Constraint picking first the white endpoint of the vertical construction line and then Shift select the midpoint of the horizontal blue line.
Dimension as shown below.
Enter d1 for both dimensions.
Notice that our geometry turns black (indicating fully defined - no more blue lines or white dots).
Remember d1 was the variable name assigned to our first dimension on the original square polygon.
Edit the vertical dimension and change to d1/2
now finish sketch.
From the Modify drop down select Split Body, select the cube as the body to split and the horizontal line as the Splitting Tool.
Attach your progress file here.
Edit Sketch1
Add the Horizontal Construction line and the Construction circle as shown.
Add the two smaller circles as shown. Add an Equal (=) constraint between the two circles.
Extrude - Joint the two circles as shown...
Change the visibility of the bodies and now Extrude-Cut the circles into the cylinder a distance of 6.5mm - this gives us a little clearance on the depth...
Now Offset face the cylindrical faces of the holes by -.1 this gives us a little clearance for the pins as we can't print perfect parts.
Add a .5 Chamfer for lead-in for the holes...
Add a .5 Chamfer to the top of the pins. This will help guide the pins for assembly.
Edit Sketch1.
Add the Vertical Construction Line as shown. Add a Sketch Point at the 12 o'clock point (I don't think we need this, but it can't hurt).
Add a Snap Fit at the Sketch Point we just created. If Fusion select any other points then Ctrl click to Unselect any other points.
Leave the setting on the default for now (I set the Plastic Rule to ABS 1.5)
Right click on the cylindrical body and set the Opacity Control to 50% so that we can see what we are doing inside the part.
