How to place a sketch plane at a specific geometric location

My background drafting is structural bridge drawings. I had Inventor LT installed the other day and I have been playing with it to refamiliarize myself with it and get used to the differences between it and AutoCAD for drawing. I found a pdf book of examples that I had been going through in AutoCAD and decided to carry on in Inventor LT. I am stuck on the following example:

I started by drawing the cross section of the rim and central hub as sketch1. I then revolved them around the central axis. I also realize I could have made a circle and extruded the central hub as another approach.

For sketch2 I drew up a view looking along the axis of the wheel.

I had three stumbling blocks in completing this.

1. The first stumbling block was the position of the R10 rib around the outside center of the center hub. The only way I have been able to position this so far would be to make it to the R13 fillet/arc between the spokes at the central hub. If this assumption is correct how do I make a plane at this point to draw the R10 circular rib?

2. The second stumbling block I have is drawing the spokes in 3D. My intent here was to draw an ellipse 22X9.5 and 24X11 at the point where the R6 and R13 curves/fillets start/end and then lofting from one to the other. Similar to my first stumbling block, how do I create sketch planes at these specific spots?

3. My third stumbling block is how to extrude/join the spoke from the ellipse to the hub or rim while respecting the R6 and R13 curves/fillets?

This is where I am currently at with the overall drawing:

Software Version: Autodesk Inventor LT 2021

Update

I figured out how to place a working plane through the R13 curve and the center of the wheel. I was then able to project the geometry of the apex of the R10 rib around the central hub. I drew a portion of a circle and on the sketch plane, and then revolved it around the central access.

Using this new ability for me to place sketch planes I then proceeded to produce a sketch plane at the start and end of the spoke where it is 22 nd 24 on the major axis and 9.5 and 11 on the minor axis.

I tried extruding with rails but that just generated errors. I also tried extruding the end of the spoke to the next object but that also gave errors. If it is actually possible to extrude the face of an existing solid, will it extrude based on its existing tapper or will it just extrude straight?

Current State:

• You can probably take it to completion by using move face to extend your spokes, and then Boolean combining them with the hub and rim - but see my recommended process below Commented Sep 17, 2021 at 12:49
• is move face the same as thicken? I could not find a move face. I also could not extrude the face of the solid without error Commented Sep 17, 2021 at 20:05
• No it's different to thicken. There is a search box in the top right you can use to search for commands! Commented Sep 18, 2021 at 7:30
• @JonathanRSwift does move face maintain the tapper? ie does the ellipse have the same dimensions at it new location, or does the ellipse shrink/grow based on the existing tapper? Commented Sep 20, 2021 at 20:23
• @JonathanRSwift found the search box in the help search box, and was able to activate the command from there but I did not have the ribbon (or part of) where it is supposed to be located. Commented Sep 20, 2021 at 20:24

tl;dr - add the fillets at the end.

Step 1: Revolve. This should also include the R10 'lump' on the central axis.

Step 2: Define the Elipse Taper. It's stated that the thickness is 11mm and 9.5mm respectively at each end of the spoke. I don't want to start this spoke at the surface of the hub as then my loft would need extending in order to fully intersect it. Instead, I will loft from the XZ plane. So, I need to know how big to make the elipse there! Create reference sketches, with the dimensioned values (11mm and 9.5mm in this view, and 22mm and 24mm in the other axis of the spoke).

Step 3: Loft. I created a plane by selecting the bottom point of my reference sketch, and the XZ plane before clicking plane. This automatically creates a plane that is parallel to the XZ plane and passes through that point. The two ellipses are easy to create by first projecting the endpoints of the reference sketches, and then making these coincident to the major and minor axes of the elipse.

Step 4: Pattern. Pattern the loft feature around the Z axis

Step 5: Cut the bore and keyway. I also champhered here since I didn't include it in the original sketch.

Step 6: Add the 3mm Fillets to the roots of the ribs (could also be in original sketch if you prefer), and then add the 6mm and 13mm fillets to the roots of the spokes

I suggest first completing your section view to include the details of the rib and the center hub, then try the 3D view again.

• I did not take the R10 rib on the spoke as being part of the one on the hub, I took those rounding marks to be the edge of the ellipse Commented Sep 16, 2021 at 17:25
• @ForwardEd Sorry, I don't follow you. Why not completing the cross-section then let's discuss. A 3D always needs a good plan view and section views.
– r13
Commented Sep 16, 2021 at 18:03

Reading this in isometric view is quite hard, I think it is better to visualize this in top, side, with cross-section view.

Anyway:

1. For the R10, I think I would try to make a plane (illustrated with black line) and create an orthogonal plane to both these plane to make a rail line and have the sketch lofted. However, it is hard to read on where the R10 center located with respect to the datum.
1. If you want to loft it, you got to make planes where the sketch will be located. It is possible to do it and I might as well approach it the same way. But to do it this way, again, we have to have the exact location on where the sketch is located with respect to the datum.

2. Don't create the fillet in sketch, use fillet feature after you extrude it and select the edges on both ends, on R6 and R13.

Does that help? I think I got it wrong somewhere, but it's because the drawing is so hard to read.

• Agreed that the center of that R13 is difficult to locate. It was not NICELY given in the original pdf sketch. I am making the assumption that it is tangent to the R10 around the central hub since I can't think of any other way positioning the R10 on the hub. Commented Sep 16, 2021 at 18:14
• How do I create a sketch plane through those end points? I also wanted to make a plane the the center of the R13 and the main wheel axis so I could sketch the R10 with its apex at the invert of the R13. When I tried lining up my two sketches which are orthogonal, I could not select any point on the other sketches line work. Commented Sep 16, 2021 at 18:18
• If you want to select point from other sketches, you have to use Project Geometry feature @ForwardEd Commented Sep 16, 2021 at 18:22
• I know how to do that in parallel planes, is it the same process for orthogonal planes? Commented Sep 16, 2021 at 18:25
• Planes need references to be created, if you have edges or sketches you can create two axis and make them a plane, its a little tricky Commented Sep 16, 2021 at 18:26

I would start from 3, ie. draw the ribs.

To do that I would first take the right plane. I would create an ellipse, and then I would extrude from the surface of the central hub to the external ring surface.

Then I would copy the rib around the axis of the wheel at 360/5= 72 degrees.

After that I would proceed to steps 1 and 2. I.e. I would select the intersection of the rib to create the radii.