How to Create Schematic Symbols in Altium Designer
What Exactly is the Schematic Symbol Generator, and Why Use It?
The schematic symbol generator tool in Altium Designer will automatically populate pins on a symbol according to a list of pins that you create. This will save you quite a bit of time if you need to place the same component multiple times.
It has a very simple interface where you can quickly specify the amount of pins and the general outline of the symbol, and then the generator will create that symbol for you. You still have the ability to manually change anything that the generator does, which you probably will want to in order to fine-tune your symbol, but the generator will do the bulk of the work for you.
To create a symbol in Altium Designer, ensure you have the schematic symbol generator extension installed and that you are currently working in a schematic. If your project doesn’t have a schematic set up, do so by going to File > New > Library > Schematic Library.
Adding a schematic in Altium Designer
To start with, you will need to add a new component in the schematic library in your Altium Designer session. For demonstration purposes, we will use a simple 74LS04 device as an example. Click on the “Add” button within the schematic library and then specify the name of the component, which in this case will be the 74LS04, as you can see in the picture below. Once the component has been added, go to Tools > Symbol Wizard to open up the symbol generator on the component.
Adding a new component symbol in Altium Designer
The Basic Operations
In the picture below, you can see the basic layout of the PCB library symbol generator. Across the top, there are settings for the pin amounts and the layout style of the symbol that you are creating. Below that is the area for editing the pins that are being added and to the right is the preview window. Note that you can control the preview window to enlarge the image.
The symbol generation tool in Altium Designer
We will change the number of pins for our symbol in a moment, but first let’s look at the layout style. Currently, the symbol is configured as a dual in-line component as you can see in the picture. Depending on what you need to create, there are several options to pick from:
- Dual in-line: Pins number top to bottom on the left side, then bottom to top on the right side
- Quad side: Pins on 4 sides of the symbol
- Connector zig-zag: Like a dual in-line but the pin numbers are numbered across from each other instead of up and down
- Connector: Like a dual in-line but the pins number from top to bottom on both sides
- Single in-line: Pins are on just one side
- Manual: You can move the pins to where you want them manually.
Although Altium Designer gives you several choices for your symbol style, for purposes of this example we will leave it set to “Dual in-line."
Next will set up how many pins are going to be in this symbol by clicking on the up-arrow. As you increase the pin numbers, the preview window will dynamically update as you go. You can see in the picture below the effect on the preview window of adding pins.
Adding pins in the symbol generator
One thing that the symbol generator has which is very useful is the ability to break-up the pins into groups. In the picture above, we have added 14-pins to our symbol and we have also broken those pins into groups. You can create groups by either copying and pasting the pins, or by specifying the name of a group in the groups column of the pin data area.
Another useful function in the schematic library and PCB library symbol generator is the ability to work within the cells of the generator as you would with a spreadsheet. The values of all of the cells (except for the position values) can be changed manually by clicking in that cell. You can also change multiple cells at the same time by selecting them all and typing in a new value. You can also paste information from another source as you can see in the picture below.
Copying and pasting pin data into the symbol generator from an outside source
In the picture above, we’ve copied some pin names and pin designators from a spreadsheet then selected the same number of cells in the symbol generator and pasted the new data in. You can see how the pin names and designators have accepted this new data, and the preview window has updated accordingly. The symbol generator also has the ability to “smart paste” data giving you control over which columns your pasted data will get copied too. This ensures proper transfer when creating the PCB footprint.
The last thing that you can change when editing pins is to set the electrical type of the pin. The default setting of the pin is as an input. You have the option though of setting it to an I/O, Output, Open Collector, Passive, HiZ, Open Emitter, and Power. These changes are reflected in the preview window with different pin graphics on the symbol.
Let’s Look at How to Create a Symbol
Now that we’ve covered the basics of the symbol generator, let’s put it to work and create our 74LS04 symbol. We’ve already got the component created and named, and we’ve already opened the symbol generator on that component. Next, let’s make sure that our pin-count is set for 14, and our layout style is set to dual in-line.
A completed 74LS04 in the symbol generator
In the picture above, you can see the symbol in the generator that we are creating. In order to get there, we need to make some manual edits to the pins. First, we need to give all of the pins their correct names from the picture of the symbol description at the top of this article. You can select each cell and type the name in or do a combination of copy and pastes. Next, we need to change the electrical type of the pins.
Some of our pins need to stay as inputs, some need to be changed to outputs, and some need to become power pins. Note in the picture above how the pin data is now sorted by the electrical type column after the changes are made.
Once you have finished your edits in the schematic library symbol editor, click on the drop-down “Place” button on the bottom of the generator window and click “Place Symbol”. This will put the symbol into your schematic. Once you’ve done this, you will be out of the generator and back in the regular schematic with the symbol that you’ve just created. At this point, you can continue to add the other parameters to your symbol.
Finishing the symbol
The symbol generator can save you time when you have to create large pin-count symbols. It is simple to use and will make your life easier. If you haven’t used it yet, take a look at it.
Altium Designer has much more functionality built into it then the symbol generator that we’ve been talking about here. Altium Designer is the complete CAD software system that you need for your PCB designs. Capabilities like the symbol generator are what sets Altium Designer apart as one of the best PCB design software tools available.
If you’ve liked what you’ve seen here and want to learn more, talk to an expert at Altium Designer to find out how you can start using Altium Designer on your next PCB design.