Hello, I'm brand new to F360 and am stuck on projecting 3 holes from one inner cylinder to an outer cylinder. I've created a cap that screws onto an inside cup and the holes will need to line up when the cap is screwed on all the way. I've tried to project the faces of the holes, but the projection is constrained to the x/y/z axis. Any help is greatly appreciated.
As currently modeled, it is not possible for the top to fit low enough on the bottom for holes to align.
In addition, the threads on the lower piece need to be chamfered in order for the top to screw on. To fix this, change the thread to not modeled, add the chamfer, change the thread back to modeled.
In order for the top to fit lower on the bottom change the start point of the threads:
Once that is fixed, use a joint to position the top on the bottom. Note: Moving the top away from the Origin is not a good practice. Leave it at the origin and turn visibility off until you are ready to position it with a joint.
p.s. It is better to use sketches to define cylinders than it is to use the primitive cylinder tool. The primitive cylinder is very lacking when it comes to parametrically modifying it.
ETFrench
@etfrench Thank you so much for the detailed reply. Your explanation was extremely helpful. I've made the corrections you suggested but have noticed the origins are not correctly aligned. Also, I'm still in need of a suggestion to extend the holes through the cap.
Recommend starting this fresh. There is too much left over baggage in the current file.
Start by drawing the profile for the bottom (Dimension and constrain all geometry).
Revolve it:
Add the un-modeled thread:
Chamfer the top, then edit the thread feature and change it to Modeled:
In order to make the top fit to the bottom of the thread, this area needs to have a relief cut which would be easiest to do in the original sketch.
I'll do another post for the top.
ETFrench
The top starts the same as the bottom and uses the same Origin. This time I added the relief for the threads😁
Since both top and bottom were modeled in place, an As Built joint can be used.
Note: 3d printed threads usually need more clearance added. One easy way to do that is to use the Offset Face command on each face of the threads. A value of -0.25mm usually works well.
ETFrench
p.s. None of this actually answered your original question, which is how to project holes from one cylinder to another. 😃 The easiest is to use the same sketch to Extrude/Cut both at the same time.
p.s. The odds of having the holes align perfectly are very low. I would make them several sizes smaller, then drill and ream them with the top screwed down on the bottom.
ETFrench
@TheCADWhisperer @etfrench Getting closer! Thank you for all of your help thus far. I started fresh making sure not to move anything away from it's origin and keeping my components organized. To get the holes, I drew both components, joined them, and put holes through both at the same time (using a circular pattern to repeat the remaining holes).
@etfrench how did you determine this dimension in the cap? I made the inner housing visible, zoomed in and placed the line's point close to but not touching the threads. Was that right?
Also, How did you make the 'relief cut'? When I go back to the sketch, I can't tell where to place the notch because the threads aren't visible.
When you apply the threads, Fusion 360 changes the original diameter to the minor or major diameter of the thread (depending on inside or outside threads), so that dimension can be anything.
Place the relief using the dimensions you set for the thread. In your previous file, that was 10mm from the top of the bottom.
ETFrench
