To create a 3D object, first you need to create a 2D sketch.
Let’s review the main functions of creating sketches. When creating geometry, the program automatically applies constraints and dependencies.
Let us adjust the settings of the applied automatic constraints.
On the Tools tab click Application options. In the window that opens, go to the tab, Sketch and set constraint inference priority to either: Parallel and perpendicular, or Horizontal and vertical.
As the dimensions in Inventor are also considered as constraints, you can select the action for over–constrained dimensions and apply driven dimension, or warn of over–constrained conditions.
We will also check Edit dimension when created.
On the tab Part by default there are specified automatic creation of sketches on the x–y plane. You may specify other planes or choose No new sketch.
We select No new sketch to specify the sketch plane manually.
Let us create the part file. Click New and specify the Default filename. We choose Standard.ipt file:
In the resulting file press the option Start 2D sketch.
Now you need to choose the plane for your sketch. In the browser area, expand the Origin folder. There you will find the planes and coordinate axis. Choose the XY plane:
Let us create a free figure of five lines, trying not to place them either horizontally or vertically, also neither parallel, nor perpendicularly to each other.
We should connect the end of the last line to the start of the first one – you will see the green dot, which means connection. Finish creating lines by pressing the Esc key.
The ends of the resulting lines are interconnected by combining dependency. We may observe it, if we press and drag any line or the end of a line.
Now let us introduce some constraints for the lines.
We set the Horizontal constraint for the lowest line.
Next – Perpendicular of the bottom and right lines.
We also set Parallel constraint for the bottom and top lines.
In addition, specify the equality of the top and bottom lines. Equality constraint specifies that stated lines will have equal length.
Specify the midpoint dependency of the right bottom point with the origin point.
The positions of the right and bottom lines are already set. That is why they changed their color to blue.
Their lengths may also change, because size constraints are not set.
Let us specify the sizes for this sketch. Select the Dimension option. You may specify the dimension of the line by clicking on the line itself, as well as on its endpoints:
Specify the dimension of the bottom line as – 30, and the right line as – 20.
Next, if we try to specify the dimensions for the top line, the program will display a notification that this dimension is not necessary, because there is an equality constraint for the top and bottom lines.
This size may be specified only as a reference.
Therefore, the constraints and position of the three lines are specified – they are displayed in blue.
Select Dimension and set the angle for the left line. To do this click on the line itself and on the bottom line. Select the position of the angle as – left, 60°.
We may also specify the size of the line in width and height, along with its length. Specify the height as equal to 15 mm.
Now the position of the sketch is fully set and all lines are in blue.
You may see all constraints by right-clicking on an empty space and selecting Show all constraints:
In addition, you may hide all constraints.
Finish the sketch and save the file as Part 1.
Close this file.
Constraints may also be applied automatically.
We create a new part and create the sketch in the XY plane.
Create a line. The start of the line should be moved to the origin until the green dot appears. This applies Combining dependency. Put the second point visually horizontally and see the horizontal constraint next to the pointer. Create a line.
Direct second line vertically to the top. You call Vertical or Perpendicular constraint, depending on the priority of constraints. We do not specify the second point and enter the length of the line on the keyboard: 50 mm.
Create an arc, the starting point of which should lay on the end of the line. Here we should specify the starting point, the end, and radius.
Close the sketch by a line.
Specify the tangency of the arc and adjacent lines.
For the left line specify vertical constraint.
Create a circle with diameter 12 mm – put a central dot and specify radius (12 mm) on the keyboard, press Enter.
Specify arc concentricity.
Draw a rectangle inside this sketch.
It already contains Parallel and Equality constraints of opposing objects, and perpendicular constraint for adjacent objects.
Specify the Vertical constraint of the middle point of the rectangle and the bottom line. The rectangle is placed symmetrically to the sketch.
For sizes, you may specify an equality using other sizes of the sketch.
Let’s specify that the width of the rectangle is equal to the arc radius.
The height of the rectangle should be equal to two diameters of the circle:
Specify that the distance from the bottom line to the rectangle is equal to the height of the top line divided by 5.
Click Finish Sketch.
Change part name to Ear and save the part.
In a sketch you may also specify chamfers and fillets.
Open our first part Part 1. In the browser area, double click on the sketch to modify it. After doing so you should see the sketch menu.
Let’s do a 5 mm chamfer for the bottom right angle:
And also a 3 mm chamfer for top right angle.
Specify fillet for the bottom left line as – radius 8 mm, and also fillet of left line – 3 mm.
You can edit chamfer sizes if needed. By doing so you change the two sizes, defining the chamfer.
Finish the sketch. Save the part.