Parts footprint, how can I edit the pads of potentiometer?
How ca I edit pads of potentiometer? The middle pad will be placed in the bottom copper, and the two side pads will be placed on top copper.
CommentsAdd a comment
Brad has given a good answer and you will probably never need to do that, just route on any side to the pad. There is quite a good book available for beginners
https://designspark.zendesk.com/hc/en-us/articles/115004904249-Is-there-a-book-about-DesignSpark-PCB- which may help you.
Also why not post in the DSPCB forum which will possibly engage more users and you can also search for keywords and find other possible useful posts and also links to the support docs.
I'm not quite sure what your question is - whether you want to change which layers the pads are present on, or change layers as you route traces to connect to the pad on a specific side of the board.
To change layers as you route traces, use the L command. (You can also change the layer of a previously drawn trace segment by clicking on it, then using the L command.)
Normally, through-hole pads on double-sided or multi-layer board have pads on both exterior layers, with plated-through holes connecting the top and bottom copper of the pads. This makes for stronger solder joints. Plated-through holes are not usually an option for people making their own boards at home, though. If that is your situation, you can solder the component lead on both sides of the board to let it make the connection through the board. There is seldom a reason to delete the copper one layer of a through-hole pad. One reason you might is to provide more clearance to route a trace between two pads of the component. More typically, I'd resize the pad instead. This is easy to do on both sides of the board. To resize on one side but not the other, I'd resize the pad to the smaller size, then I'd add a filled shape (circle) on the side where I want the larger pad, overlapping the smaller pad to expand it.
To change the size of a pad or change if from all layers to a single layer, right-click on the pad and select Properties...
Then click on the Pad tab of the Properties dialog.
You should then see something like the attached image.
You need to check the Pad Style Exception box before it will let you modify the pad on a component already on the board.
You can then change the size, shape, and layer(s) of the pad.
@BradLevy Good day sir, I just happen to see some tone controls of famous companies that their potentiometer's center pad was placed at the bottom copper and their two side pads is in the top copper.
@yeng-yeng, In most cases it will make little difference which side of the board the trace is run on. If the pads are close together, starting half of the traces on the opposite layer of the board (top vs bottom) may give you more room to jog the traces around obstacles, but it depends on what else is on the board and how crowded the board is overall. There are some cases that call for careful trace placement on different sides, and sometimes additional measures as well. These reasons come to mind: Isolation of hazardous voltages. Safety standards sometimes require that portions of the circuit that are potentially at high voltages have at least a certain minimum clearance from system ground and user interfaces. That is why you see some optoisolators in curiously long or wide packages. The package is intentionally made large enough to meet the clearance distances that some of the safety standards demand. In other cases, the circuit may be amplifying very low-level, high-impedance signals, which can be disrupted by leakage currents. Some real-time-clock circuits operate at extremely low currents in order to maximize battery life when power is absent. Keeping those leads away from other traces, and sometimes taking the additional step of applying a moisture-proof conformal coating to that part of the circuit helps keep the leakage currents down. Sometimes very intentional trace routing is used to keep sensitive traces from running parallel and near to high-frequency or high power drive signals that could inductively or capacitively couple noise into the more sensitive circuit. And in very high speed signals, traces may be routed very specifically to match the delay between two traces of a transmission line. In an audio amplifier, preventing noise from being coupled into lines in the input stage is probably the most likely reason for any very specific trace routing.