To facilitate drawing in the sketch, you can right-click on the navigation cube and click on Show the normal of the sketch plane. The 3D view will rotate to place you in front of the sketch plane in progress.
Creating your first part in OnShape
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OnShape (2) - Your First Part
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Pré-requis :
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Objective:
The objective of this tutorial is to discover the basic functions of OnShape by step-by-step creating the part shown above. All the functions used are not exhaustively explained, so feel free to test some options yourself.
Creating Your Project
STEP 1
In the top left corner, click on the Create button and then on Document
STEP 2
Give a name to your document and then click on OK
STEP 3
You should be redirected directly to the main page of your part editor. Make sure you can navigate correctly in your 3D space with your mouse before continuing.
Overview of the Window
General View
The design window is divided into 4 areas:
- Area 1: 3D/2D view of the part
- Area 2: Tabs for parts and project elements
- Area 3: Function and part tree
- Area 4: Toolbar
1 - 3D/2D View
Area 1 is dedicated to the 3D and 2D view of your part. In 3D view, you can navigate around your part and select the elements to interact with. You also have access to the navigation cube allowing you to manage your display and its orientation very quickly.
2 - Part and Project Element Tabs
The different parts you create and open will appear in the tabs below your window.
You can add elements to the project by clicking on the + button to the right of the tabs.
3 - Function and Part Tree
On the right, you will find the display area for the function and part tree. It details all the parts of your project (at the bottom) as well as all the functions of your current part (at the top). For better readability, you can hide this area by clicking on the button 
.
4 - Toolbar
At the top of your screen, you will find the toolbar that gives you access to the functions that allow you to create and manage your parts.
This toolbar can be configured by going to My Account (click at the top right on your account) > Preferences.
Creating Your First Part
STEP 1: Create a Sketch
Go to the toolbar and click on Sketch 
.
Select the Top plane as the sketch plane (double-click on the plane in question). Your selected plane should appear in your sketch window:
STEP 2: Create a Rectangle
Go to the toolbar and click on Rectangle by Corners
.
Draw a rectangle around the origin point as shown in the image by clicking once to define the first corner and a second time to determine the second corner. Do not click and pull (click-drag)
STEP 3: Center Your Rectangle
There are several methods to center your rectangle on the origin of your part. Read both methods carefully and test:
Method 1: by Midpoint
The square being centered on the origin (a point), click on two end vertices of the square and lastly on the origin point.
Then click on Midpoint in the constraint toolbar 
.
Method 2: by Symmetry
You can also center the square using double symmetry. Click on two opposite vertices of the square and then on the line separating them:
Then click on Symmetric 
.
Repeat the operation for two other vertices.
STEP 4: Equalize the Sides of Your Rectangle
Select two adjacent sides of your square, then click on Equal.
STEP 5: Dimension the Sides of Your Square
Click on the Dimension tool 
then select one of the sides of your square. Enter the value 30mm to fix your side to a dimension of 30mm.
WARNING
Note how your sketch has gone from Blue to Black. This means that your sketch is fully constrained. It is important to ALWAYS check that your sketches are fully constrained before exiting a sketch and continuing your work.
If this is not done, you may find yourself in situations where your futur part generation will break if you edit a previous sketch that is not fully constrained.
STEP 6: Validate and Exit the Sketch
If you are satisfied with your sketch, you can exit it by clicking on the Validate button 
. You then exit the sketch mode and return to the 3D view. You can switch back to a trigonometric view by clicking on one of the corners of the navigation cube 
STEP 7: Create an Extrusion
Select your previously created sketch
then click on Extrude 
in the toolbar. In the menu that appears, make sure to select New and Blind, then change the value to 10mm.
Then Validate to exit.
STEP 8: Create a Second Sketch
Click on Sketch then double-click on the right plane to validate it as the sketch plane. Remember that you can right-click on the navigation cube to orient your view (Show the normal of the sketch plane).
STEP 9: Quick Sketch of Your Shape
Make a quick sketch of the desired shape (see illustration) using the Line tool 
.
INFO
When you create a complex sketch, a simple and effective method in most cases is to:
- Make an unconstrained sketch of your sketch
- Geometrically constrain your piece using constraint tools
- Finish by dimensioning the sketch
- Check that your sketch is fully constrained This is the method you followed to create the base of your piece, and it is also the method we will use for the second part of the piece.
STEP 10: Dimensionally Constrain the Sketch
Using the Dimension tool 
, dimension as indicated the sketch you previously created. Check that your sketch is fully constrained, then Validate to exit.
STEP 11: Revolved Extrusion
Click on the Revolve tool 
then select your previously created sketch as Faces and sketch areas to sweep. Then click on Axis of Revolution 
and select the edge of the sketch around which we will perform our revolution. Make sure the Add tab is active.
Then Validate to exit.
STEP 12: Drilling Sketch
Create a sketch on the top plane (Top) and reproduce the sketch opposite using the Center Circle tool 
. Constrain the elements as seen previously, then Validate to exit.
STEP 13: Material Removal
Select your new sketch created earlier, then click on Extrude 
. In the window that appears, select the Remove tab 
, then in the End Type, select Through All 
.
If the direction of material removal is not correct, you can reverse it using the Opposite Direction button 
. Then Validate to exit.
STEP 14: Circular Repetition
Click on the drop-down menu next to Linear Repetition and select Circular Repetition.
In the Piece Repetition drop-down menu, select Function Repetition. Indeed, what we are going to repeat circularly will be the material removal function performed earlier for our drilling.
In Functions to Repeat, select your previous extrusion (the drilling) and in Repetition Axis, select one of the cylindrical surfaces at the center of the piece created earlier using the revolution tool.
Set the instance counter to 6, then Validate to exit.
STEP 15: Chamfers and Fillets
Click on the Chamfer tool 
then in Entities to Chamfer, select the edges you want to chamfer.
Set a distance of 3mm for your chamfers, then Validate to exit.
You can do the same with the Fillet tool 
by selecting the base edge of the cylinder.
Modifying Your Part
CAD tools are inherently parametric tools. This means that they allow you to make modifications to your parts by going back through your construction tree. This allows you to correct or add elements to your part by going back up your tree without having to redo your entire design.
For example, in our case, we will make several modifications:
MOD 1: Base Dimension
In this first modification, we will change the size of the sketch, and then we will modify the height of the base.
Double-click on your first sketch (the one for your base). You will return to Sketch Editing mode for your base. Change the dimension of your square side to 40mm 
, then Validate to exit.
To modify your base height, double-click on the extrusion of your base in the construction tree, and change the height to 5mm, then Validate to exit.
MOD 2: Hole Dimensions
Double-click on the hole sketch to enter edit mode, and change the circle diameter to 4mm and the distance from the center to 16mm, then Validate to exit.
MOD 3: Number of Holes
Double-click on the circular repetition function, then change the Instance Counter to 4 instances. Finally, Validate to exit.
