Servo Motor Mount

The procedure follows that of the introduction to Fusion 360, Rather than select a circle a rectangle is selected.

Selecting rectangle will present the sketch palette that includes a rectangle. In the first option two corners of the rectangle must be specified while in the third the centre point and one corner. The third option is chosen.
Note the snap to grid option is set .

To form the rectangle click on drawing origin and one corner. The proposed dimensions are 50x35. However since snap to grid is set the final dimensions are 50x36.

To complete 2D drawing right click and choose OK.

To generate the 3D base select Finish Sketch, in the tool bar select Extrude.

The display should be set to 3D view of Home.

The extrude will give a number of options. In this example the starting point will be the Profile Plane which is XY as defined as the first step in creating the sketch. There is then a choice of extruding one side, two sides or symmetric One side is chosen. The next step is the distance to extrude. Minus 2 mm is chosen to take the extrusion below the profile plane. This will allow additional objects to be placed on the base to start at the profile plane.ie Z=0

Upon extruding the next step is to add 4 mounting holes. For this step go to top view. select create sketch and move to top view.Draw a centre rectangle (40x26) using the construction option. See earlier screen Linetype

Right click and select OK.The construction lines are difficult to see but corners will be where the mounting holes go

For ease of locating holes use the point option in the Create (Sketch) mode. Place point at every corner of the construction rectangle. They will snap to grid.

Go to solid mode and select hole.

Once the hole is selected the next step is to select the plane (In this example the XY (Red Green). Once this selected a hole symbol appears

There will also be the Hole Palette.

From the Hole Palette for placement select the second option Multiple Holes

To generate the holes click on each point in turn. The previously defined parameters will be used. When complete click OK.

On the TOP view Create Sketch and draw a rectangle. Do not worry about the sizes. DO NOT press OK.

Go to the Dimension tool by pressing D. The rectangle dimensions can be set by selecting an edge and inserting the desired size in the inverse video box. A few enters on the keyboard might be necessary.

To position the rectangle select edge of base and rectangle and enter value. Some cursor movement may be required to select measurement of concern.

When done press Finish Sketch

To generate the upright select SOLID then extrude and select rectangle (Shown in blue).

Enter a distance of 25mm of 25mm for the extrude. This will be from the profile plane. (Recall earlier the base was extruded below profile plane)

Press OK. By default the new object will join the base plate.  

With the FRONT view chosen select Create Sketch and use the line tool draw the servo support. The horizontal distance is approximately 12 mm and the vertical 10mm. The other dimensions are left arbitrary to illustrate dimensioning angles. 

Any angles close to 90degrees Fusion will constrain them to 90 degrees

Do not press finish sketch.

To dimension the angle first use the "D" command and click on the sloping line. Moving the cursor will give the line length and its projection.

Now click on thr short vertical line and the dimension shown is the angle. Adjust this as required (120 degrees shown) 

Note as the dimension is changed the node remains fixed.

Press finish sketch

The sketch should be observed at different angles to see the sketch reference for the support.

To extrude select Solid, Extrude and the support sketch.

In the Extrude palette select symmetric direction and either set the distance or use the arrow in the sketch. When satisfied press join and OK. 

Portion of the support part of the model must be cut. In the TOP view draw a rectangle from the edge of the support to the upright. Use the D command to dimension what will be the parts of the support remaining.

After finishing sketch select Extrude then the new rectangle and in the Extrude Palate select CUT. By using the arrow in the diagram the depth of cut can be dimensioned. Note before hitting OK it is educational to observe the model in different views. 

Press OK when satisfied.