Modelling products, machines or other stuff in SolidWorks is just as in the real world. First you’ve got to build several parts before you can assemble all this parts in one product. You can put multiple parts together in SolidWorks with an Assembly. When this job is done and the virtual product is ready you can create your own drawings which can be used for the production of the parts and products.
This tutorial is about how to start with your first part.
Before you start with this tutorial it’s recommended to read 0. SolidWorks introduction.
When you would like to create a new file choose: File-New or press ‘Ctrl + n’ on your keyboard. You’ll get a popup window where you can select the type of file. We start with a part file.
When you create a 3D part in SolidWorks you just have to remember that you always begin with a 2D sketch which is similar to AutoCAD, Photoshop, Illustrator or other 2D orientated programs. Start with a basic shape and add slowly more detail to it to have always the control to edit what you need to edit.
Choose new part in the option list (The assembly and drawing will be discussed on later posts).
Create a Sketch
The way of building your model is very easy. Just create a 2D sketch and add features to this sketch to make it a 3D model. This 3D model is called ‘a solid’, a closed object.
To create your first sketch just select the front plane in the feature tree and a small quick menu appears. Click on the sketch icon to add a new sketch to the front plane.
And choose ‘Sketch’ by clicking on the sketch icon.
The command manager has two basic and some advanced tabs. The two basic tabs are the sketch and feature tab. In most situations the sketch commands are shown automatically. In case they’re not; go to the sketch tab in the command manager and all the sketch commands are shown in the toolbar.
When you start with a sketch two buttons are shown in the right upper corner of the graphic area. In this triangle you see two icons. One icon to apply all the changes and the other one to discard the changes.
When you look at the feature tree you see that sketch1 is added.
Click on the rectangle in the sketch command toolbar.
Click on the origin to prevent it from floating in the space. Drag the mouse to create the rectangle and click to accept the rectangle. Do not mention the size yet.
You can always use the ‘escape’ button to reset your command. The default selection arrow appears.
Smart Dimension
Now we add some dimensions to the rectangle. We use always ‘Smart dimension’ to add a dimension to the sketch.
Click on the left vertical line to add a dimension. Click another time next to the line to apply the smart dimension.
When you click for the second time a small ‘Modify’ window pops up and here you can add your value. Type in you keyboard ’120′.
Use the middle mousewheel to zoom the entire sketch.
Add a dimension of 120 to one of the other horizontal lines.
Mention the fully defined mark at the bottom of the interface, the status toolbar. This means that the sketch has references to the origin and all the lines are provided with a dimension. When you drag a point this has no effect to the sketch! Make sure that all your sketches are fully defined.
Note!
A lot of AutoCAD users are used to add the dimensions of a rectangle to the property manager. This is not the way to work with SolidWorks because the dimensions are not stored in the sketch and the sketch is still under defined. Also do not use the fix button. This will fix a line and prevent dimensioning the sketch.
If the rectangle isn’t black after you’ve added the dimensions, please check if the shape is fixed to the origin correctly. Select a point and drag the point to the origin.
Apply the sketch by clicking on the apply button in the upper right corder of the graphic area.
Add a Feature
The next step is to make a solid block of the sketch. The way to do this is by adding the feature ‘Extrude’ while the sketch is still selected (in this case Sketch1 is highlighted, blue). A feature is a one of the commands to make your solid form a 2D sketch.
You see the feature tab is visible on the left upper corner of the interface. Select Extrude.
The sketch turns a couple degrees and you can see a yellow solid with an arrow in it. You can drag this arrow to apply the dimension or you can add a value in the box on the left. Add a value of 50mm to it.
If you want do cancel this operation you can hit the ‘Esc’ button or just click at the red cross above the properties. You can apply these changes to click on the green ok button. These buttons are also in the upper right corner of the graphic area.
Now you’ve got a solid block! It looks just great, doesn’t it? Play a little bit with the zoom (scrollwheel) and rotate function (press the scrollwheel and drag the mouse). You zoom the part on the place where you’ve got your cursor.
Edit Sketch
You can edit your sketch by right clicking on the sketch.
Now you see the first sketch on the same angle you saw the block. You can see the icons at the upper right corner of the graphic area. This means you’re in a sketch.
Edit the dimensions by double clicking on the dimensions and add a value of 100mm.
If you would like to see the sketch full frontal you can change the view with the standard views. Choose front to rotate to the front plane and zoom the sketch to the window (remember that we’ve made the first sketch on the front plane).
Now change the other dimension to 100mm.
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Apply these changes by clicking on the apply button in the upper right corner.
Now we’ve got the same model, but different dimensions. Mention that we still look at the front plane!
Edit Feature
Now we’re going to adjust the depth of the block by editing the extrude feature. There are two way’s to edit the dimension.
The first one is by right clicking the extrude feature in the feature tree and choose ‘Edit Feature’.
Change the properties to your desired dimension. In this case choose a dimension of 80mm and click on the Ok or Apply button in the upper right corner.
The second way of editing the dimension of the extrusion is by double clicking on the model after you’ve rotated it a bit to see all the dimensions. The black dimensions are the sketch dimensions, the blue ones are feature dimensions.
You see al the dimensions who are related to the solid. Just double click at the depth (50), change this dimension to 80mm and hit the ‘Enter’ button or click Apply.
You will return to the solid block and you will see no changes to the dimensions of the block.
Rebuild button
Hit the rebuild button to rebuild the block. All the changes you’ve added will be added to the visual model.
File storage
I recommend logic file names for the files you are creating. An assembly contains a lot of parts so choose your file names logically! For example: make use of project numbers, part numbers and maybe a module character.
Folder 09001 Project Example – Project number project description
900101 Example box top.sldprt – Project number Part number Part description
0900102 Example box bottom.sldprt – Project number Part number Part description
For this example I give the file the name: part1. The extension .sldprt is automatically added to the file.
Another Sketch
Now we add the cylinder to the top of the part. You can add a new sketch to the solid on two different ways.
Select the front surface of the model, not the front plane, and a popup window shows up.
The other way is to select the front plane and go to the command manager. Select the sketch tab and choose ‘Sketch’.
Now you’ve created a new sketch on the front surface of the solid block. Look at the feature tree and the upper right corner. You’re in a sketch!
Sketch the circle on the block. Choose the circle command in the command bar and select randomly the centre on the block. Click again on a random spot to set the diameter of the circle.
Add a dimension to the circle with smart dimension. The desired diameter is 70mm
Note!
Don’t insert your dimensions in the lower properties bar like you do in AutoCAD. These values are not stored in the part and don’t create a situation where the sketch is fully defined! Also don’t use the fix option. This is not a flexible way to add relations to your sketches!
The circle is still blue which means that the sketch is not fully defined. Add smart dimensions from the centre of the circle to the outer edges of the block.
Insert a value of 50mm to both edges.
Note!
When you’re new to SolidWorks you may have the problem that you see a dimension between hooks: (dimension). In this case you’ve added a dimension when you were not editing the sketch. Delete all this dimensions and add the dimensions in the sketch.
Aplly the sketch and go to the feature command bar.
Select ‘Extrude’ while sketch2 is selected to make the cilinder.
Give cylinder a depth of 30mm. Make notion to the direction of the extrusion.
You can see that there is a new feature added in the feature tree. There are two extrusions. Sometimes in large parts you can choose to add a more sufficient name to the feature. In this case I named the two features ‘Block’ and ‘Cilinder’. Just double click slowly on the features in the feature tree.
The next step is to add a hole in the cylinder. Select the top surface of the cylinder and add a new sketch.
Draw a circle with a diameter of 50mm. We’re going to add a relation to the new circle and the existing cylinder. Select the circle and the edge of the cylinder and a pop-up window shows up. Click on the ‘Concentric’ in the pop-up window or the property manager. In both cases you only see the available relations. In this case the known ‘vertical’ or ‘horizontal’ relations aren’t shown in the list.
The sketch is fully defined.
To make the hole you’ll have to apply the sketch and go to the feature command manager. Select ‘Extruded Cut’.
You could add a value to make a hole trough the whole solid but it is easier to select ‘Trough All’
Apply the feature with the green Apply buttons.
Sometimes the extruded cut goes to the wrong direction. It’s a matter of changing the direction to solve this problem. Press the button ‘Reverse direction’.
Our part to this far.
Now it’s time to create some smooth edges to the solid. For the best results: create the large fillets first!
You can specify the radius of the fillet. Sometimes you’ll get an error message because the radius is larger than the dimensions of the model (in this case larger than 100mm). In this case I choose a radius of 10mm. Select the edges you would like to fillet. You’ll have to turn the solid to select all the edges. If you click twice on one of the edges the fillet will not be applied to the edge.
All the selected edges are shown in the list under the radius box.
Press the apply button.
You can also select a surface to add a fillet.
A chamfer is a oblique modification of a solid part.
Select the top surface and modify the feature properties.
Press Apply to submit the feature. Look at the difference between a fillet and a chamfer.
At last I’m going to make a shell of this solid part.
Select the bottom the the part and set the thickness to 2mm
Okay, now I’ve got this part:
Change the dimensions of the first sketch to 120×120. The extrusion has to be 30mm. This is one of the powers of a 3D CAD program!
At last we add some colour to this part. Select the file (file name) in the feature tree.
The result
Go to the next tutorial: 2. SolidWorks Drawing basics
