I think i have almost all of the Gerber files for making a double-sided PCB that has parts on both sides. But, as i vaguely remember, there are some companion files: Pick-and-Place that give part designations like R1..R23 1K2 1/8W IRC film etc, part placement like R1 Xnn Ynn C23 Xnn Ynn etc . I think there were three. How can i generate those?
Thanks.
Found the missing file types i need to generate. Made a sample to show what i need to make:
Pick & Place generated by WinBoard V2.10 Date Created: 7/1/2006
Components Pick & Place Report File: G:PCB.PIK
SMT components on the component side
File: PCB.pk1
Component Count
-------------------- MMDT2222A-7-F 39 CRCW06030000Z0EA 1 VJ0603A181JXBAC 1
Adhesive locations on the component side
File: PCB.pk2
SMT Components (Component Side) Report File: PCB.pk1 (partial, sample)
Q1 MMDT2222A-7-F 0.1206 0.2376 0.00 Q2 MMDT2222A-7-F 0.2456 0.2376 0.00 Q3 MMDT2222A-7-F 0.3474 0.2376 0.00 Q4 MMDT2222A-7-F 0.4806 0.2376 0.00 (etc) J1 CRCW06030000Z0EA 2.2344 0.0335 0.00 C1 VJ0603A181JXBAC 1.2345 0.4015 0.00
Adhesive (Component Side) Report File: PCB.pk2 (partial, sample)
0.1206 0.2376 0.0394 0.2456 0.2376 0.0394 0.3474 0.2376 0.0394 0.4806 0.2376 0.0394 (etc) 2.2344 0.0335 0.0125 (faked) 1.2345 0.4015 0.0125 (faked)Bill Of Material Report File: PCB.BOM (partial, sample)
Count Component Type Module Type Component Reference
----- ---------------- --------------- --------------------- 1 CRCW06030000Z0EA 0603 J1 39 MMDT2222A-7-F SOT-363 Q1 Q2 Q3 Q4 (etc) 1 VJ0603A181JXBAC 0603 C1
We generate them from the component source file. The actual file format does not really matter. Any good assembly house can write the proper filter to parse your files. All they want is your data, since they don't want to be blamed for mistakes.
Ther is a ULP on the Eagle site that can generate the Centroid data.
Cheers
I'm still running Eagle 5.11 To generate the placement files and bill of material, I use an external ulp called bom-am-xx
I just use the output section and have two setup files. One gives placement information and the other gives bom information. I generate in html format which mystifies most people. First, it prints nicely because of the formatting. Second, the contract manufacturer can import the html format into Excel very nicely.
If anybody wants the setup files, email me at oppie dot bob at gmail dot com.
All gerbers are >> I think i have almost all of the Gerber files for making a double-sided
Not as distributed; had to ask a PCB maker to send me one. By the way, there seems to be TWO "standards" for pick and place: one using center of package, and another using the "center" of pin one foot; neither with no regard to shape or size of package. So on has to guess which "standard" the assy house uses..
Thanks.
Using center of part when you make a library component makes it simple for the placement data. You may have to offset this slightly to make sure that all pins wind up on the routing grid.
I have used several turnkey vendors for board fab/assembly. None had any problems with my methods.
Oppie
btw- I put the bom-am-19 setup files I use >> >>
Check; the ulp i got from Screeming Circuits uses the centroid. Nobody else has complained. I made a ulp from that one to create the pk1 file in same format as from Ivex WinBoard. Took me a while, as i am not a "C" guy and we do not get along with each other (at least 2 orders of magnitude worse tan Word).
Speaking about the two apparently independent languages as used by Eagle (ulp, scr), could something be written to convert a library package layout to a text form for DECENT and EASY modification, and another to convert back? Ivex had a very nice program they named "MCL" that looked at the file type for conversion.
Oh, yes, that leads me to a pet peeve. It seems impossible to take a library package layout and modify it for a new, ADDED part in the library. Likewise, it is impossible to "break out" one as a separate part for editing, and ASS-u-ME-ing one had such a beast, then INSERTING / ADDING to the library. Naturally, the "help" documents are useless here - so what else is new, this kind of documentation standard has been made famous by none other than the prestigious Microsoft.
You can make a library from a board. Place the part on a board, then make a library from the board. I think there is a ulp for that inthe ulp dir.
Cheers
If you need to modify a library part, copy it or better yet, copy the symbol and footprint with new names, edit as necessary and then define new part using these. I have a link on my desktop to the eagledata directory so I can do things through windows that Eagle doesn't normally support. Whenever I need to look at library files, best to do it in the Eagle control panel first. In the control panel, browse to the libraries. You can easily go through the library and see what parts are available and display in the right hand panel. In left hand panel, if you right click on a part, you get options to add to schematic, add to brd or, if you have a library open already, copy to library. This is for Eagle 5. Haven't tried Eagle 6 yet (everything changed to XML and once a drawing is opened, it is converted to new format and you can't go back...)
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.