I would like to make one component with multiple footprints.

I realize diptrace cannot exactly do this, but what is the best practice to work around this?

I created a part atmega1284p pid component, labeled all of the pins as needed. works great
I copied the component to a atmega1284p qftp tried to map the pins to the part. All looks good on the component and the pint mapper.

However, when I place the new item on the pc board, the pin mapping wants to use the mapping from the original (pid)- all pins are not correct.

I am assuming I messed up someplace, but not sure where.

I could not find any documentation on this topic. Is there any docs or best practices for this?

thx

(moved from wrong topic)

Hmmm...I do this quite often: build a component in Component Editor, with an attached footprint. When that part is done, I right-click on the part in the column at the left side of the Component Editor window, select "duplicate part", then select that part (right below the first one in the column). Rename it (in the Component Properties window)...of course, it must have a different name than the first one (usually just the suffix that indicates the package). Click on "Pattern" at the bottom-left of the Component Properties window for the new part. The "Attached Pattern" window opens. Open the appropriate library at the lower right of the Attached Pattern window, and select the new pattern for the new part. Check that all the pins are connected correctly: sometimes the new pattern won't have quite the same pin numbering, depending on the part. Click OK when done. Be sure to SAVE the component library.

Maybe there are other ways, but the above way has worked well for me, and I've never had any trouble getting the right footprints associated with the various versions of the component. Of course, it also works for simple parts like diodes and resistors and capacitors that can all have the same schematic symbol, but come in various packages. You can also use that method to create, for example, a series of the 0805 resistor values you have in stock; you can make the value visible by default, and have specific part numbers associated with each component in the list if you want.

This is the method I tried. For the most part was successful but here was where my issue came in.

Create a part (atmega1284 PDIP pattern). Name all of the pins, as desired, design and build board. So far, good.
Copy the part and rename atmega1284 qtfp. Go from a 2 sided part to quad, go from a 40 pin to 44 pin

Go to the original board - replace part with the qtfp part. If I do a new board with the new part, it seems to work - only the replace seems to mess me up.

Now the schematic comes up with the new part, everything looks good (connection names, etc look good), create a new board and all of the pins are if the original still existed. Example, the crystal get connected to pins 12 & 13 (the pdipd pattern), but the schematic showed it coming in on the pin labeled xtal1 & xtal2 which are on pins 7 & 8 on the qtfp part.

I guess what I was expecting that the replace would use pin names, not pin numbers.
My only solution was to delete the part, then add it new, reassign all of the pins and it seemed to work.

However, I might be totally missing some easy way to manage this.


BTW - This is not a complaint, just would like to know what are the best ways to handle this. This product has a few items that don't quite work as I would like, but coming from eagle, these are minor issues. I can live with the issue as long as I know it will happen.

I'm not sure I completely understand, but maybe I know what's going on. I just had a similar issue with pins on a much smaller part. If you haven't done it yet, try this: instead of just "replacing" the component on the schematic, FIRST disconnect it (right-click on component, select Disconnect Wires), then "replace" it, then connect it ("Connect Wires"). I assume that your replacement schematic symbol is identical for both parts, just that the replacement has different pin numbers.

Please let us know if that works better for you.

Example: I make a simple circuit with a 2N2218 NPN transistor. The emitter is pin 1, the base pin 2 and the collector pin 3. If I "replace" the transistor with an MMBT2222LT1 from the Motorola library, which has pin 1 as base, pin 2 as emitter, and pin 3 as collector, the schematic wires move around so what used to be connected to the emitter is now connected to the base, and vice-versa. However, if I first disconnect the wires from the transistor, then replace it, then reconnect the wires, they are connected properly.

This will likely work as it is the same as deleting the part and re-adding the new one with the new footprint. With 44 pins or more, I was trying to save some time and potential errors of not adding the correct signal to a pin.

Ah, but if you delete the part without first disconnecting the wires, the wires connecting to the part will also disappear. If you disconnect wires, replace part (with one with an identical symbol, or at least with identical pin positions and origin), connect wires, then there is nothing more to do, no wires to replace. If you disconnect, delete, add part -- you have to position the part correctly. If you just replace, the symbol will appear in exactly the same place as the original. That seems a bit safer to me, and a bit easier. But of course you are right, you can accomplish the replacement by deleting the original and placing the new part.

Good point. However when I have a part with many wires, I generally just add to net and connect without wires. Otherwise the schematic gets to messy. So in this case, would not help much.