Work with 2D sketchДмитрий Зиновьев
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.
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:
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.
Now let us introduce some constraints for the lines.
We set the Horizontal constraint for the lowest line.
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.
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:
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.
Finish the sketch and save the file as Part 1.
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.
Specify the tangency of the arc and adjacent lines.
Create a circle with diameter 12 mm – put a central dot and specify radius (12 mm) on the keyboard, press Enter.
Specify arc concentricity.
It already contains Parallel and Equality constraints of opposing objects, and perpendicular constraint for adjacent objects.
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.
Click Finish Sketch.
Change part name to Ear and save the part.
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.
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.