Welcome to the CADSTARguys Blog - Information, hints, tips and my waffle on the CADSTAR Printed Circuit Board design suite.

Please note that all names used are completely fictitious and any thing written is my own personal opinion or knowledge and not related in any way to either my employers or their customers (or Zuken).
Also this is not a replacement for proper Maintenence/support and you should read the help files before asking anything techy:).

Saturday, 29 June 2013

Component with multiple pads/same connection.

I was recently asked how to make a component footprint for the inductor here and this applies to any component with a similar component footprint.

It is an inductor where the datasheet asks for 2 long pads but with only the ends of the pads being exposed for soldering to.
The question was - How to do this ?

If you look at the footprint information supplied:

You can see from this footprint that the shaded area (which is solder resist) effectively separates the 2 long pads into 4 smaller exposed pads where each pair are joined together under the resist.

This can easily be achieved in CADSTAR by adding 4 pads and connecting them together using component copper, I shall show you how.

First figure out from the drawing how big the 4 pads need to be and add 4 rectangular pads so that the left 2 are pads 1 and 3, the right 2 are pads 2 and 4 as follows.
(The reason for this is that the inductor symbol has only 2 terminals so you can identify them as pads 1 and 2.)

Then add some component copper that covers pads from pad 3 down to pad 1 and from pad 4 down to pad 2 as follows.


That will provide you with the required 2 large copper pads but with 4 exposed areas, however as far as your netlist goes pads 1 and 2 are connected to your circuit, pads 3 and 4 are not and you will get component copper to pad errors.

To prevent these errors and connect pads 1 and 3 together with the copper, in the copper properties enter the pad numbers (identifiers) for both pads.


What this will do is electrically connect them together, so in the part you only need to allocate pin 1 and 2, then when connecting to pin 1 - pin 3 is connected via the copper (Max pins = 2).

You can only connect 2 pads together like this so if you are wanting to connect more than 2 together you simply use more pieces of component copper and daisy chain them together etc.

So you will end up (once you have added the outlines etc) with a component footprint that looks like:



Finish the component off with Placement, silkscreen and assembly outlines - origins etc. and your component is ready to be made into a part.

For similar components - perhaps where the datasheet calls for a pad shape not supported by CADSTAR, you can create the shape with component copper and attach it to a pad that covers as much of it as you can, 99 out of 100 time this is more than adequate for the component.

Any problems - post a comment.

Addendum.....
When creating the symbol it must have only 2 terminals, using 4 will enable you to add 4 nets to it in the schematic and in the PCB it will need to be only 2 - 4 will produce an error.

7 comments:

Abu Abacus said...

Is this apply to SOT223 packages too ? E.g.: linear regulators such as LT1117 ?
With Pulsonix it is possible to assign a logic pin to more than one physical pins. I was not able to find this functionality in CADSTAR :(

thanks

The CADSTAR Guy's Blog. said...

No, this only applies when a copper connection is required between the 2 pads.
In that case, the component copper can join 2 pads together to the same net.

If you want SOT233 pins 2 and 4 to both be on the same signal then simply add both pins to the symbol and connect them both in the schematic.

Abu Abacus said...

Thanks for the answer. It is sad anyway. In this case I have to add a new pin in the symbol.... thanks anyway

The CADSTAR Guy's Blog. said...

You do not need to add any more pins in the schematic symbol - read what I said above.

Abu Abacus said...

Thanks...

Another question which is related to this one I think.

I'm creating a new component. For a simplicity let it be an operational amplifier. On the schematic symbol I don't want to have pins for power connections e.g.: VCC and VEE. When I create a part from it, I can assign a net to a footprint's pin, in the Signal column in the part definition. So let pin 4 connected to a signal called VEE, and pin 7 to VCC.
When I put 2 of this part on schematic, and export it to pcb editor, then I can see the connections between the power pins.

My question is. What if I would like to use different power for these two components ? Let's say VCC1,VEE1 for the first one, and VCC2,VEE2 for the second ?

Ok, I can add power connections on the sch symbol, but I don't want them. Consider an FPGA chip whit many power pins. I would like to connect the power pins of different FPGAs to different power nets.

Is there any method, to redefine the 'Signal' assignments (which is defined in the part definition) in schematic editor or somewhere else ? The schematic editor doesn't see these nets, but the constraint editor does (I assume it is reading it from the part definition, while sch editor doesn't). If the value which is defined in the Signal column (part definition) cannot be changed later, then it has not much use for me. But it is hard to believe, I think I just didn't find it how :(

thanks

The CADSTAR Guy's Blog. said...

In a word - no.

You are suggesting explicit pin/net names but want to change them.

If you define the signal name on a pin in the part, this pin name is not visible or changeable in the design, in fact if you do not have that signal available then the pin is not connected. This is the way it used to be for the older 74 series IC's etc however modern devices need more pins on different nets and its far better for them to be available in the design.

Add the power pins to a power block which you can put on another sheet so they are still available yet do not need to be part of the main schematic. Although not having the pins visible to the reader makes it problematic as they wont know what pin does what.

This is why explicit pins is a legacy feature that is little used now and I would certainly not be using it in a FPGA chipped design.

Abu Abacus said...

Thak you for the answer

Post a Comment