I Cannot Set a Layer for a Test Point Pad...Follow article
The DesignSpark PCB software support community is there for you if you need help with issues that might just stop you finalising your electronic circuit designs. It could be that you can’t find the right component footprint, or you just can’t get your head around certain software functionality. Whatever the issue there’s bound to be someone who can answer your call for help.
One of our DesignSpark PCB users had an issue trying to set a layer for a test point he had created within his design, he asked for help, and it arrived, read what happened below...
I Cannot Set a Layer for a Test Point Pad...
I created a one pad component called test point which is a rectangular bare pad and it works fine except I get a track to pad error if I put this pad on the top layer and there are bottom tracks underneath. Looking at pad properties I see that the pad is set to layer [All] and I cannot change it in properties or using the L key
How do I fix this so I behaves like a normal SMD pad?
Hi Bill, not sure why you have that behaviour, but another issue you will face is solder paste on the pad. Have a look at https://designspark.zendesk.com/hc/en-us/articles/115003349025-How-can-I-add-a-fiducial-mark-to-my-PCB- which shows how to get a copper area (pad) without solder paste and should not have the issue you are experiencing.
Bill, I take it you were trying to change it from [All] layers to [Top] layer by editing the properties of the pad in the PCB editor after placing the component on your PCB. You can (if you check the Pad Exception box in the properties editor) change the style of the pad, but not its type (through-hole vs SMD, which is controlled by the Layer: setting).
The way to fix it is open the library manager (ctrl-L), and edit the PCB Symbol you are using for your Test Pad component. The PCB symbol editor does let you select the Layer assignment for the pad. If you change it to [Top], it will be on the top layer when you later place the component on the PCB. Once it is on your PCB, you can use the Flip command to flip it from the top side to the bottom side of the PCB.
If you need a component that is in some cases through-hole and other cases surface mount, you can define two PCB Symbols (one through-hole, one surface mount), and define the Component in the library as having two available packages, one using the through-hole PCB Symbol, and the other using the surface mount PCB Symbol.
As Boss pointed out, though, if you want a test point without solder paste, you need to create the test point as a shape on the copper layer and a corresponding shape on the solder mask layer. Unlike a fiducial which you usually don't connect to a net, you do want your test point connected to a net. You can make a PCB Symbol like the following:
Where the highlighted white rectangle is an actual pad, and the red is a shape on the copper layer, and the same red shape is copied to the solder mask layer of the symbol. (You'd need to include a solder mask layer in your design technology of the PCB Symbol, and also in the design technology of the board you are placing the test points on.
The red portion then gives you a test point without solder paste (so you get good contact), and the highlighted pad gives you a place to connect the pad to a net. You can make the rectangle (which will have solder paste) smaller if you want.
The one disadvantage to the test points is that you will get a design rule check error about the pad overlapping the shape. You can safely ignore the error because you know the overlap was intentional in this case. But it would be nice if we could turn off that message on a per-PCB-Symbol basis.
Thanks for the tips - Brad's tip to edit the component fixed my problem and I actually prefer that test points get solder on them since it helps probes dig in so they don't slide around when using the test point.