Keep Your Altium Designer PCB Layout in Line with Grids and Grid-Selection Shortcuts
Table of Contents
The grid system in a printed circuit board design CAD program is a great tool for a PCB designer, and it's a system worth knowing. Altium Designer® has a well designed grid system that you can use to your advantage in your PCB designs and schematic captures. Before all the different snap and placement utilities that are now available in CAD systems, we used to have to constantly manipulate the grid to place objects at different locations.
It seems more for designers to have adopted the attitude of “set it and forget it” when it comes to their grids. Grids are still important, perhaps now more than ever, and learning to use the grid to your advantage can be a real benefit to you.
Altium Designer has a Unified Cursor-Snap System to give you precise control over your main grid, and the ability to set-up and control many other grids as well. With this system of multiple grids, you don’t have to constantly reset your main grid. On the other hand, if you prefer working with one main grid there are easy ways to do that too. This system has several features, and work in both the layout and schematic views.
Altium Designer provides you with the main default grid, the Global Board Snap Grid, as well as the ability to create additional grids that you can use for specific purposes. The core of this grid system is the PCB grid manager. This is the utility that allows you to create and delete additional grids as well as set up and control any grids that you will use during your design session.
The key here is to make sure that you don’t have anything else selected in the design session when you click on the properties button, or you will get a menu for the selected object’s properties instead of the board properties. Once the “Properties” menu is open, scroll down until you get to the “Grid Manager” section in the menu.
Use the “Panels” button to access the “Properties” menu, and scroll down for the Grid Manager
The “Global Board Snap Grid” is the main default grid in Altium Designer. Although you can change the parameters of this grid and enable or disable its use, you aren’t allowed to delete it. Notice in the image above that when first opening the grid manager, the only grid listed is the main global board snap grid. By selecting this grid and clicking the “Properties” button within the grid manager window, you can adjust the parameters.
You can do all of your design work by manipulating the main global board snap grid, or you can create additional grids for different purposes.
To create a new grid, click the “Add” button within the grid manager window and select “Add Cartesian Grid” from the pop-up menu. Note that a new grid has been added to the PCB grid manager named “New Cartesian Grid”. Select it and click the properties button to open up the Cartesian Grid Editor. This editor allows you to set up the different parameters as shown in the image below.
Changing the parameters of a new grid with the Cartesian Grid Editor
The Cartesian Grid Editor gives you a lot of control over your grid set up. Here are a few of the parameters that you can alter:
- The name of your grid: You can change your grid to a more descriptive name.
- The units of the grid: You can choose between metric and imperial.
- The steps of the grid: Here is where you will set up the grid spacing; 1mil, 5mil, 25mil, etc.
- The size of the grid: How large of an area do you want this grid to cover?
- The display of the grid: This is where you will set the color and step multiplier of the grid, as well as whether the grid will display in dots or lines.
There are many other options here as well. The X & Y values of the steps and the extents can be linked or set separately depending on your needs. There are also controls for the grid origin and quadrants. In the image above, you can see where the display color was selected opening a “Choose Color” submenu. Here you can choose between standard or custom grid colors.
Once the grid parameters have been set, click “OK” to close the Cartesian Grid Editor.
In the image below you can see the addition of two new grids to the Circuit Board grid manager. Each grid has a priority number to the left of its name. This priority is what will determine which grid is displayed in your design session. You can also change it by right-clicking on the grid to adjust its priority level. The global board snap grid has the lowest priority level preset to 50 which can’t be changed.
Multiple grids shown within the grid manager
To control which grid is to be displayed and used, enable or disable the “Comp” and/or “Non Comp” buttons to the right of each grid. By enabling “Comp”, the grid can be used for component placement while enabling “Non Comp” will allow you to use the grid for everything else. When moving components, a “Comp” enabled grid will display even if it is a lower priority than other “Non Comp” grids.
Many years ago I laid out round boards that were used for IC testers that required components to be spaced on equal radiuses. This was before CAD systems had polar grids and our ad hoc system was a painful process of drawing lines on the radiuses by manipulating the regular grid system and using a lot of math. Then to place the you had to set the grid to the smallest value possible and eyeball the component to land on the radial lines that we had drawn.
Altium Designer gives you the ability to add a polar grid
Fortunately, Altium Designer has provided a solution to this by giving you the ability to create a polar grid. From the Circuit Board grid manager, you will go through the same steps to create a new grid only this time you will select “Add Polar Grid” as shown in the image above. The same controls for priority and comp or non comp apply to a polar grid as they do for a cartesian grid.
The Polar Grid Editor gives you the same control over your grid as the Cartesian Grid Editor does, although some of the settings are specific for the polar grid. As shown below, you have the ability to control angular ranges and radial ranges instead of extents and quadrants.
The Polar Grid Editor menu in Altium Designer
You may not have a lot of use for a polar grid depending on the technology that you are designing for, but if that need comes up you will be very grateful for this grid in Altium Designer. Even boards that aren’t “round” may still require electrical components placed on a radial grid, and Altium Designer has that need covered for you.
Altium Designer with a polar grid displayed
Many renowned self-help books will tell you that there aren’t any shortcuts in life, but these people never laid out a printed circuit board. Fortunately, Altium Designer is loaded with keyboard shortcuts that you can use to your advantage. Here are some of those shorts to help as you work with Altium Designer’s grid system.
Pressing a “G” on your keyboard will bring up a list of preset global board snap grids
When you are in Altium Designer, pressing the keyboard shortcut of “G” will bring up a list of preset grid values as shown in the image above. This will allow you to quickly set the global board snap grid to any value in the list by simply clicking on it. This menu will also give you the option of going into the cartesian grid editor for the global board snap grid as well as manually setting the snap grid value.
Other keyboard shortcuts include “GX” and “GY” which will allow you to set individual grid values for either the X or the Y values. Another shortcut is “Ctrl+G” which will bring up the cartesian grid editor for the global board snap grid. The most used shortcut is probably “Shift+Ctrl+G”. This little jewel will bring up a small dialog box which will allow you to manually enter the value you want for the global board snap grid.
Using grid control keyboard shortcuts can save you lots of time while working on your design
Altium Designer comes complete with many different utilities such as the grid system that we’ve been discussing here. These functions and shortcuts truly position Altium Designer as one of the best PCB design software tools and schematic creators that you will find. Even something as simple as setting a grid has been enhanced to give you the maximum performance in order to best help you to complete your designs ahead of schedule and under budget. When you need the best layout tools to help you stay productive, look to the complete set of PCB design features in Altium Designer®. In addition to the best PCB layout and routing features, all users have access to an Altium 365™ workspace, where it's easy to collaborate, share projects, and release files to a manufacturer.
We have only scratched the surface of what’s possible with Altium Designer on Altium 365. Start your free trial of Altium Designer + Altium 365 today.