Hello, how can I create a "connected jumper". It is a mixture of using a starpoint but with 2 pad, which are connected by default without getting DRC errors.
The idea behind is to have a measurement connection without using the same netname but have it closed by default. -> For the first prototypes I can scratch the connection, and later on for series production it will stay connected, so I don't have to change the design anymore. I do not know how this is called in english.
I'd perhaps create it as a new type of star point. You can add your own types of star point. You can use define pad style to edit a rectagular pad to thin it out in the middle by making to opposite cut ins to get a single pad dumb bell or dog bone shaped.
Thanks for the advice, I got some steps further ( however this was a lot of trial and error ) This is what I got so far, a star point where I could use an alternate pad style of style type "special" which I designed by Setup->Define Pad Shape ( in the PCB Editor ).
Image Insert: 15.75 KB
After conneting and some routing trials, I found that there is no DRC error on this:
Image Insert: 11.28 KB
hm, I will continue. What do you think of using this "Wire" Feature? Could this be a solution? I had no luck with it up to now, but maybe I am just missing how to use it for SMT pads.
Your pictures look like what I was trying to explain. The wires layers aren't really suitable for what you are after since they don't give you a physical copper pattern and the net name is the same both sides. They are used for insulated or non-insulated wire links across the pub for a single net. If you use them and output an ipc-d-356 netlist then your pub fabricator should come back to you with queries about open circuit nets when they check the imported Gerber and manufactured board against the netlist. Some people use the wire layers to connect pads in footprints that use the same net such as a sot-223 heatsink pin or a fuse holder with two legs but there are other (better?) ways of achieving this.
ok, I finally found a workaround, which has all the features I wanted to have. I created a block including 2 starpoints with a net connecting it internally. Also I created a nice symbol for the block. After translating this to the PCB, I moved the 2 starpoints nearby, routed the net and created a tight group with these 3 elements. Advantage: In schematic the block looks like a device and can be reused and multi instanced. In PCB it is a litte manual work at the moment ( as do not know how to create and use prerouted blocks ) but after grouping, you see that both nets stay at their own pad.
Cool solution, I like it. You could create it in a schematic and a con and add to your library and use apply layout pattern the next time to save time placing and routing it in the new pcb.
Posted - 29 Dec 2016 : 19:17:03
