I read once that circuit board design is 90% placement and 10% routing. I’m not sure that I believe that, but it is fair to say that component placement is a critical part of the overall board design. Yet some designers will rush this part of the job so that they can get on with routing the board, only to have to come back later and re-place portions of the board.
I wonder if one of the problems is that designers get frustrated during the Altium component placement process. It does take some time to get all of your components correctly located, aligned, and positioned so as to provide the most optimum routing channels. This is especially true if you are working with design tools that are limited in their placement capabilities, or if you just don’t understand the placement functionality that you have available in your design tools that can help.
Fortunately, Altium Designer® has some powerful placement functionality that can make your job a lot easier. There are manual placement utilities to help with alignment, and you have the option of organizing your components for placement by selecting them first in the schematic. Also, if you need some help in finding and selecting specific components for placement, there’s a utility for that as well.
Use the Alignment Feature to Straighten Out Your Placement
I must admit, having to constantly move components around during placement can be annoying. I have often had a string of components lined up just the way that I want them, only to discover that a new component needs to be squeezed in. Once I move everything around to get the new part in, my perfect alignment is now shot and I have to tweak all the components to get them lined up again.
Yes, manually moving each part it is a straightforward operation, but wouldn’t you agree that if there was some simple help available that it would be nice to use?
Altium 18 has this help ready for you to use in its placement alignment tools. There is a whole menu of different alignment functions at your disposal, and here is an example of how you can use them. You will notice in this first screen capture that I have a row of misaligned components that needs to be cleaned up. There are even some clearance violations between pins that are too close together.
Components that are not aligned
First I selected all of these components and then used my right mouse button to get to the “Align” menu. Once I was in the Align menu, I selected “Align” from the top of the list to pop up the “Align Objects” sub-menu that you see below.
Set your alignment parameters
In the “Align Objects” sub-menu I selected the parameters that you see above. For my horizontal alignment, I directed Altium to give the components equal spacing. For my vertical alignment I elected to align by their tops, and then I clicked “OK.” As you can see below, my components are now aligned equally the way that I want them to be.
Your components are now aligned as you want them to be
This is not a feature that you will use every day, but when you have a row of components that need to be quickly cleaned up, this can be very useful. The key to getting the most out of a feature like this is to become familiar with it so that it is second nature to you when you need it.
I have talked with many designers that have simply never taken the time to learn how to use all of the help that their design tools provide for them. Because of this, they miss out on functionality that is intended to help them. This alignment tool in Altium Designer can be a very handy tool to keep in your back pocket, use it.
Altium Placement Cross-Select Mode from the Schematic
Aligning your components is a great feature to use once your are placed on the board, but I know a lot of designers that struggle just with getting started on their placement. Having a bunch of components outside the circuit board outline with connections going everywhere can be a daunting puzzle to try to plow through. Again though, Altium Designer has a utility in place that will help you with this.
By going into the schematic, you can select groups of circuitry that need to be placed together on the board. Once selected in the schematic, you can then designate a rectangle in the layout where you want those selected components to be placed. This allows you to quickly organize the components in your layout by how they are drawn in the schematic which in turn will facilitate a better placement on the printed circuit board.
With the components spread around the exterior of the circuit board outline in layout, I opened the schematic to the sheet that I needed for a group of connected circuitry. I then went to the menu; “Tools > Cross Select Mode” as shown in the picture below.
Use the Cross Select Mode in the schematic
Next, I selected the components that I wanted to be placed in the schematic sheet by dragging a select box around them. You can see in the picture below the selected components in the upper half of the schematic sheet.
Select the components for placement in the schematic
After activating the layout window, I next selected the menu item; “Tools > Component Placement > Arrange Within Rectangle” as shown in the picture below. The cursor in the layout window will show as a green crosshair indicating that it is ready for the placement rectangle to be specified. Click to establish the first corner of the rectangle, and then click again for the opposite corner.
In layout, select the Arrange Within Rectangle function
After creating the rectangle in the center of the printed circuit board outline, Altium Designer populated that area with the selected components from the schematic. You can see the components that were moved into that area in the picture below.
The selected components in the schematic place their counterparts in layout
This won’t be the placement that you stay with, you will still have to move the parts around to optimize their final placement on the board. This is a very good way though to group together connected circuitry from the schematic without having to go through and identify and move each component individually. This trick alone can save you a lot of time during placement by allowing you to organize your placement based on how the circuitry is drawn in the schematic.
Place Individual Components Using Choose Component
When it comes time to moving individual components around, you can position the cursor on the component and hold the left mouse button down to move the component. Did you know though that you can also type in the shortcut “m” to get into the Move menu?
Once in that menu, you will find different move commands that you can use. One of those commands is “Component”, which will pop up a dialog box allowing you to select by reference designator the component that you want to move.
AltiumComponent placement with one component missing
In the picture above I wanted to find and place the component U89. I typed in the shortcut “mc” (Move Component) and then clicked in an empty area of the board. This brought up the “Choose Component” menu that you see in the picture below. Note that I have the option to select the component from a list, or to type in the reference designator at the top. I also have the option to jump to the component or to move the component to my cursor.
The Choose Component menu in layout
After selecting U89 from the list I chose the option that moved the component to my cursor and clicked OK. With U89 on my cursor, I was able to easily place it into position as you can see below.
Component placement with the missing component placed
This feature will save you a lot of time when you need to find a specific part of placement. Instead of searching through the schematic, or looking at all of the parts scattered around the board perimeter, you can simply select the reference designator and place the component.
Altium Designer 18 has many more time-saving features built into it making it the premier PCB design software tool. With placement aids such as what I’ve shown you here, your focus can be on creating the best placement possible instead of trying to figure out how to manipulate the design tools.
If you’re not already using it, talk to an expert at Altium to find out more about how Altium Designer 18 can help you with your next PCB design.
About the AuthorVisit Website More Content by Altium Designer