Acquiring and Adding libraries to ExpressPCB and other programs.

[Jrd]

I am currently trying to work with ExpressPCB but the component library is so limited, I am trying to add the transformer from the RenSS boards Mouser# 838-3FS-312 (http://www.mouser.com/ProductDetail/Tamura/3FS-312/?qs=dKoSqUwwxaVVFhKoQs6fZw%3d%3d) Manufacturer# 3FS-312 but it is not in the list. Where can I get more libraries for ExpressPCB and how do I install them?

Thanks

[Matt_Edwards]

I can't help you with ExpressPCB libraries , but I find the only libraries I trust are the ones I make myself. Most of the time you can trust the libraries supplied with the software, however RPM's recent experience has not been so fortunate.

[dirknerkle]

I am currently trying to work with ExpressPCB but the component library is so limited, I am trying to add the transformer from the RenSS boards Mouser# 838-3FS-312 (http://www.mouser.com/ProductDetail/Tamura/3FS-312/?qs=dKoSqUwwxaVVFhKoQs6fZw%3d%3d) Manufacturer# 3FS-312 but it is not in the list. Where can I get more libraries for ExpressPCB and how do I install them?

Thanks

Essentially, you make those components yourself. I've done it many, many times and all it takes is a little time, trial-and-error and a printer. You design the part and then do a test print. You usually have to move one or more mounting holes a bit, but when you print it out, you can check the printout against either the part itself or a board that has that part. You just line up the holes. When you have a perfect match, you save the part in your "custom components" for use at a later date.

It's easy to do...

[n1ist]

That transformer is quite easy to make a model for. Just 6 holes. The diameter isn't specified, but the pins measure .0.046" on the diagonal (Pythagorean Theorem to get this based on the pin sizes given). I'd use the 0.056" hole with 0.115" pad since it's a heavy part. Pick an empty point on the board and move the origin to that point (View->Set origin with mouse). Hole spacings are given, so you can just double-click on the pads and type in the coordinates, and give them proper pin numbers. Then draw the outline rectangle on the silkscreen (yellow) layer. Select all the pads and the outline, group them, and save the new component.

I would also make a schematic symbol for the transformer; in this case, I'd start with the existing transformer, ungroup it to allow editing, and then regroup and save when done.

Here's my models for this part.
10589
/mike

[Jrd]

Thanks for the replies guys.

I can't help you with ExpressPCB libraries , but I find the only libraries I trust are the ones I make myself. Most of the time you can trust the libraries supplied with the software, however RPM's recent experience has not been so fortunate.

Ouch, what software was he using?
I have Eagle and Kicad also but this file is in ExpressPCB format.

Essentially, you make those components yourself. I've done it many, many times and all it takes is a little time, trial-and-error and a printer. You design the part and then do a test print. You usually have to move one or more mounting holes a bit, but when you print it out, you can check the printout against either the part itself or a board that has that part. You just line up the holes. When you have a perfect match, you save the part in your "custom components" for use at a later date.

It's easy to do...

So we have to make most of the renard components and other things we may want. I sometimes get ideas for things I could put to use but haven't found a program that has the right parts and I don't have many of the parts I would need to base a component off of, I naively thought that there would be a program that has most components.

That transformer is quite easy to make a model for. Just 6 holes. The diameter isn't specified, but the pins measure .0.046" on the diagonal (Pythagorean Theorem to get this based on the pin sizes given). I'd use the 0.056" hole with 0.115" pad since it's a heavy part. Pick an empty point on the board and move the origin to that point (View->Set origin with mouse). Hole spacings are given, so you can just double-click on the pads and type in the coordinates, and give them proper pin numbers. Then draw the outline rectangle on the silkscreen (yellow) layer. Select all the pads and the outline, group them, and save the new component.

I would also make a schematic symbol for the transformer; in this case, I'd start with the existing transformer, ungroup it to allow editing, and then regroup and save when done.

Here's my models for this part.
10589
/mike

Thanks Mike, that helps for this project, it seems I'll have to make most of the components for other projects though.

What if we had a thread where members of DIYC could post their libraries? I'm sure we could trust libraries from members who design boards like Dirk, Budude, Phil, Wayne, etc.

[n1ist]

If someone posts an ExpressPCB board or schematic, you can always save individual components from it to your library. Most other CAD packages (Kicad, PADS, Allegro) let you do the same. I think Eagle also does, but I haven't used it.

Libraries is a perennial problem with CAD packages; even the ones costing many thousands of dollars have the same issue. Unless the part is very complex, I find it usually faster to create my own model rather than hunting and verifying ones from the web.

Posting libraries of common components (or the schematic and board files to grab them from) is a good idea; have you checked the copper section of the library here for boards that use the same parts?
/mike

[Jrd]

No, I never thought about harvesting parts and honestly don't know how to do it.

[dirknerkle]

No, I never thought about harvesting parts and honestly don't know how to do it.

In ExpressPCB, it's easy.

1. Load the PCB file into the editor.
2. Select one of the components.
3. Click COMPONENT in the menu bar
4. Choose "Save Custom Component"
5. Give the component a descriptive name
6. Click Save.

[Jrd]

Thanks Dirk.

It says: "Can not save the selected component, one or more of it's pads are connected to a power plane. Right click on each of these pads and select no connections." This comes up for most of the components on the low voltage side of the miniren84XB especially the XBee and PIC. If I right click on a pad I do not see a "no connections" option.

Got any ideas? Thanks.

[dirknerkle]

Thanks Dirk.

It says: "Can not save the selected component, one or more of it's pads are connected to a power plane. Right click on each of these pads and select no connections." This comes up for most of the components on the low voltage side of the miniren84XB especially the XBee and PIC. If I right click on a pad I do not see a "no connections" option.

Got any ideas? Thanks.

Right-click on what is probably the ground pin on the component, and choose Bottom Layer Pad Shape. It probably will have one of the thermal plane options checked. Set it to NONE to disconnect it from the ground plane. Then you can save it.

[Jrd]

Thanks, that does the trick.

[buckanear]

There is an ExpressPCB group in Yahoo that has a sizable library. Again it caveat emptor

james