| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

7. Tutorial (continued)

7.6 Placing Parts

In this section, we will place the parts on our PCB.

- Set the Placement grid to a reasonable value such as 100 mils for placing the through-hole parts, which have a pin spacing of 100 mils. This will make it easier to align the parts. Later, we may use a smaller grid for the surface-mount parts.
- Select Show all from the View menu (or press the "Home" key) so that you can see all of the parts. It will help if you make the FreePCB window as large as possible (although then you may have trouble seeing this tutorial, unless you have dual monitors).
- Before placing any parts, take a minute to review the schematic. If you haven't already done it, it may be useful to print the schematic so that you can refer to it while designing the PCB. Since U1 is the largest and most "connected" part, I would suggest placing it somewhere near the center of the board, with the other IC's near it. The headers JP1-JP6 should probably be placed near the edges.
- Let's start by placing U1. Select it by clicking on it. A white outline should appear around the part, indicating that it has been selected. Be careful not to click on one of the pads or the reference designator, or you will select that instead of the entire part. If you are having trouble finding U1, you can use View > Show part to select it by reference designator.
- Tip: Sometimes it can be difficult to select a small part that has relatively large pads, such as a surface-mount capacitor. However, here is a trick that you can use. FreePCB will never select something that is already selected, if there is an alternative. Therefore, if you click on a part and select a pad instead (or any overlapping structure), just click again and you will usually get the part. You have to be sure to allow enough time between clicks that Windows doesn't mistake your two clicks for a double-click, which usually doesn't do anything.
- With U1 selected, press F4 to begin moving it. Drag it towards the center of the board. The cursor will be "attached" to pin 1 of the part. Rotate it by pressing F3 once, so that it is vertical with pin 1 in the upper left corner. When it is near the center of the board, left-click to place it. It should look something like:

- Notice that the ratlines moved with the part. After you placed it, you might have noticed that some of the ratlines changed their pin connections. This is because FreePCB automatically optimizes the ratlines for minimum total length after moving a part.
- Now let's place the other DIP ICs, U1 and Y1, something like this:

- Now place the DIP headers around the edges of the board, something like:

- As you place the parts, it is a good idea to look at the ratlines to try to find an optimal placement for easy routing. However, you don't necessarily have to see at ALL of the ratlines. On this board, we will be using internal power and ground planes for the VCC and GND nets. Therefore, we might as well make the ratlines for these nets invisible
- Select Nets... from the Project menu. The following dialog should appear:

- Most of the dialog is occupied by a list of all of the nets. The number of pins and the trace and via widths for each net are shown next to the net name. Also, to the left of each name is a checkbox, which determines the visibility of the net ratlines. Currently, all nets are visible. To make the VCC and GND nets invisible, uncheck the boxes next to them. Then click OK. Now there are fewer ratlines visible.

- Now place the rest of the parts. As mentioned above, selecting some of the smaller surface-mount capacitors may be tricky, unless you place the cursor precisely between the pads, or use the two-click method. You may want to use a smaller Placement grid, such as 50 mils. As you place each part, you may have to move the other parts around to make room or to improve the efficiency of the connections. Try not to crowd things too much. On a real-life densely populated board, the parts placement may be critical to successful routing, so it pays to take the time to get it right. That shouldn't be much of a problem on this board, however.
- You can see my final parts placement below. Note that I moved U2 to the right of U1 to shorten the ratlines between these parts.

- Now, let's position the reference designators for the parts on the silk-screen layer, so they will be correctly oriented and visible when the parts are soldered on. First, set the Placement grid to a small value, such as 10 mils, for finer control of the placement of these small items. Select each reference designator by clicking on it, and move it with the F4 key. As with parts, F3 rotates the reference designator while dragging.
- Since the reference designators for the mounting holes aren't very useful, you can make them invisible by selecting them and pressing F5 ("Set Size"), and then setting their size to zero. Since they are positioned directly over the pads for the mounting holes, you probably won't be able to select them by clicking on them, since you will get either the part or the pin instead. Therefore, use the selection mask to disable selection of parts and/or pins, and then click on the reference designator. Alternatively, with the mounting hole part selected, select Set Ref. Text Size from the right-click menu. This is also how you would make them visible again by increasing their size.
- Here is the final screenshot.

PREV | Table of Contents | NEXT