Total 3D Newbie Question

larry_athey

I will start off by saying that my only computer drawing/diagramming experience is in the 2D world using basic programs such as Dia and Gimp under Linux. So, it's safe to say that things in the 3D world are not obvious to me.

Now, I'm not looking for somebody to hold my hand, I'm just looking for examples that I can watch and then use that as a guide to get me where I need to be. What I need to 3D print is something very similar to a 4" PVC 45 degree Y coupler where the 45 degree connection is a 2" connection. That's just what it's similar too, going to a hardware store and just buying one isn't going to get me what I need.

I have watched a number of Onshape tutorials and I have yet to find one that shows something like joining two pipes together at a 45 degree angle. Go ahead and laugh, but all I've managed to figure out so far is how to make a 4" pipe that is 4" long and has 1/8" thick walls. How to join a 2" pipe of the same wall thickness to the side of it at a 45 degree angle and punch a hole through the side of the 4" pipe is totally escaping me.

Can anybody point me towards some tutorials showing me anything that would get me down the road?

Jake_Rosenfeld

Hi Larry,

I went ahead and made a simple mockup of what you wanted so you could see one approach to making it (by no means is this the right/only way).

https://cad.onshape.com/documents/0d5c6922517bbba54cec90a5/w/7c5e47c5000b33eb5c47ed2d/e/852a6d3044cd0abd5e63dd70

What I did was:

1. Made the original pipe by extruding the area between 4-inch and 4 1/8-inch sketch circles
2. Added a "Offset" plane halfway up the pipe
3. Drew a line tangent to the pipe on this plane
4. Added a "Line Angle" plane  using the tangent line and a 45 degree angle
5. Sketched a 2-inch and a 2 1/8-inch circle on the 45 degree plane
6. Extruded those circles into another pipe (using the "Add" option in the dialog so the two pipes would join into one part).
7. Extruded the inner circle of the original 4 inch pipe using the "Remove" option in the dialog so that it would remove the excess pipe material created by the 2 inch extrude
8. Extruded the inner circle of the 2 inch pipe using the "Remove" option in the dialog so that it would punch a hole in the side of the 4 inch pipe.

Feel free to copy this document; I expect this isn't exactly what you want, but I think that if you use the rollback bar to look how it was made one step at a time and double click the features to see what kind of parameters I used you will have a good idea of how to make something similar for yourself.

Armindilo

Like Jake_Rosenfeld said, there is no right way and there is no 'only way'. Just to show you, here is how I would approach this part:

https://cad.onshape.com/documents/f6fec9930959f5e092add16f/w/cd8884dce5ef97e6734a4977/e/651a8e3cd8465d8cbf73b4ef

1. Make the main 4" pipe using a revolve feature. (sketch is on the front plane)
2. Make the secondary 2" pipe using a revolve feature. Make sure your feature is set to 'Add' not 'New'. (sketch is on the front plane as well)
3. Use the shell, specify your wall thickness, and select areas you want to remain open - in this case select the 3 places where the pipes enter.

Each method has it's pros and cons, and there are probably a hundred other ways that you could do this. The approach you take will be largely determined by your experience, your 'design intent', and your personal preferences. Take a good look at these examples and get a thorough understanding of how each of them functions. Keep it up! And keep asking questions!

Jake_Rosenfeld

Nice design Armindilo! Definitely a lot less complex than my 45 degree planes.

Jake_Rosenfeld

Hi Larry,

I went ahead and made a simple mockup of what you wanted so you could see one approach to making it (by no means is this the right/only way).

https://cad.onshape.com/documents/0d5c6922517bbba54cec90a5/w/7c5e47c5000b33eb5c47ed2d/e/852a6d3044cd0abd5e63dd70

What I did was:

1. Made the original pipe by extruding the area between 4-inch and 4 1/8-inch sketch circles
2. Added a "Offset" plane halfway up the pipe
3. Drew a line tangent to the pipe on this plane
4. Added a "Line Angle" plane  using the tangent line and a 45 degree angle
5. Sketched a 2-inch and a 2 1/8-inch circle on the 45 degree plane
6. Extruded those circles into another pipe (using the "Add" option in the dialog so the two pipes would join into one part).
7. Extruded the inner circle of the original 4 inch pipe using the "Remove" option in the dialog so that it would remove the excess pipe material created by the 2 inch extrude
8. Extruded the inner circle of the 2 inch pipe using the "Remove" option in the dialog so that it would punch a hole in the side of the 4 inch pipe.

Feel free to copy this document; I expect this isn't exactly what you want, but I think that if you use the rollback bar to look how it was made one step at a time and double click the features to see what kind of parameters I used you will have a good idea of how to make something similar for yourself.

TimRice

Great write up Jake! @larry_athey if you get stuck along the way feel free to make the doc public and post a link to the document here. You''ll find that many people here on the forum are quite helpful.

Armindilo

Like Jake_Rosenfeld said, there is no right way and there is no 'only way'. Just to show you, here is how I would approach this part:

https://cad.onshape.com/documents/f6fec9930959f5e092add16f/w/cd8884dce5ef97e6734a4977/e/651a8e3cd8465d8cbf73b4ef

1. Make the main 4" pipe using a revolve feature. (sketch is on the front plane)
2. Make the secondary 2" pipe using a revolve feature. Make sure your feature is set to 'Add' not 'New'. (sketch is on the front plane as well)
3. Use the shell, specify your wall thickness, and select areas you want to remain open - in this case select the 3 places where the pipes enter.

Each method has it's pros and cons, and there are probably a hundred other ways that you could do this. The approach you take will be largely determined by your experience, your 'design intent', and your personal preferences. Take a good look at these examples and get a thorough understanding of how each of them functions. Keep it up! And keep asking questions!

Jake_Rosenfeld

Nice design Armindilo! Definitely a lot less complex than my 45 degree planes.

larry_athey

Thanks a million for the example and the cheat-sheet to duplicate it. I think that one of the biggest stumbling blocks for me here is the terminology used in Onshape and I don't know if this terminology extends to the rest of the CAD world. I will tinker with things and see where I get. Thanks again!

larry_athey

OK, one more quick question. The bottom of the 4" pipe...If I wanted to make that smaller in diameter in order to be able to stack these on top of each other, would that normally be done by making another extruded part and mating it to the bottom of this, or is it possible to actually shrink the diameter of the bottom of the pipe?

bruce_williams

@larry_athey  Least steps would be to follow @Armindilo  #1 making the main pipe sketch including the smaller end (and radii if you wish) and revolve would.    Or you could Add  with an Extrude or Revolve but that is more steps.  There is no way to just 'shrink' the end.

Armindilo

You could add another extrude to the bottom of it. I would do it before the 'Shell' feature to maintain consistent shell thickness, but depending on your design you may want different thicknesses.

As before, there are multiple correct ways to do it: I would modify 'Sketch 1' to have a narrower section at the bottom. I've copied my original example here to demonstrate:

https://cad.onshape.com/documents/f6fec9930959f5e092add16f/w/cd8884dce5ef97e6734a4977/e/6ba02fc8205a4094e46ba226

Edit: updated URL.

larry_athey

Well, I got it (kinda)...Just curious, why is the extruded part that I added to the bottom a different color from the rest of it? Does that indicate that they aren't all one solid part?

https://cad.onshape.com/documents/5859790b51077710486a8f8b/w/716cb9afff0a0d9bead7f527/e/1192545ab01868826d3c1fee

Hakro

@larry_athey:
Beside Part1 you created Part2 in the PartStudio. New parts get allways a new colour. You can use "Edit appearance" to change the color.



Or do you want only one part inside the PartStudio? Then you have to edit "Extrude5" and switch from "New" to "Add" and select Part1 as "Merge scope". But that will not work because there is a gap between the two parts. Error: "Boolean resulted in no geometry change. The parts either do not intersect or are totally contained."

larry_athey

Looks like I answered my own question. They are two parts since the ID of the original part is 4.00 inches and the OD of the other part is 3.99 inches. Boolean union won't work, but changing either diameter won't allow them to be stacked (I still wonder if .01 inch difference between the two is enough in reality).