BGA's from viewlogic

[Carl_at_xrite]

Help!!
I had this problem some time ago and now I have it again.
When I create a bga in viewdraw I assign the alphanumeric pin numbers a1,a2 etc. and create a Powerpcb decal/part with the same alphanumerics .
When I link the schematic and pull the parts into the board the pins are no longer in order on the bga.
What gives? Is there an easier way to do this?
I really want my symbols to match the spec. sheets.
Thanks in Advance.
Carl

[Lameris]

First, submit an enhancement request for PowerPCB 6 so that DECALS support Alpha-numeric pins without requiring part type mapping!

Is Viewdraw putting it's own PowerPCB parttype in the PowerPCB libary? Or do you have another Parttype in a earlier search parth. This happens automatically when the interface creates the .p file which is then imported into the PowerPCB "usr" library. Delete/backup any of the Viewdraw created files, parts and decals and then see if the pin numbers match! You may need to update the part in ECO... Do a search for the Parttype in all libaries.

Second PowerPCB enhancement request! Alias's are required for both parttypes and decals in PowerPCB so that we get the component specified by the schematic from the proper library. If the partype or decal is later changed in ECO by the designer, it is cool, but simply finding a wrong part because it is first identical name in the search path is unacceptable. (I don't know how many 1206, DIP8, etc. decals are in our libraries, except that there are too many)

Third method, add a Viewdraw pin file or PINORDER attribute. Check with techsupport on how to create one. I think pin files are a poor method to fix the problem, mostly because of the Viewdraw file bloat, I am afraid of deleting a required file.

I hope this gets you started...
Gary Lameris

[Carl_at_xrite]

Gary,
All components are entered through DXDataBook except for mounting holes etc. so the pkg_type and device are based upon my DxDatabook entries.
I created a "decal" in pads and saved the alphanumerics to the part type called out by "Device" in DxDatabook I also do not allow Viewdraw to overwrite my part libraries during the link process.

I had tried an experiment and added the pinorder attribute with no labels listed and the pin order worked okay but, now that the component is in a schematic I can't link to a board due to the missing labels in the pinorder attribute.

I guess I am stuck with having to add the pinorder to the BGA parts but what a hassle when you name and number each pin and then have to enter all the information again.
I'll have to look into the pin file maybe I can "cheat" through Excel
Thanks Gary.
Carl

[Lameris]

You can export the Parttype from PowerPCB and then use that to create a pin file as described from the Veiwdraw help below.

To create a pin order file:
1. Using any text editor, create a file using the .pin file extension in the sym
subdirectory.
2. List the pin labels in the appropriate pin order, separating the pin labels
with a space (or place them on separate lines).
3. Save and exit the file.

This is what the Exported Parttype file should look like from PowerPCB. Lines 4+ are decal pins 1,2,3,4,5 etc. It should be simple to create a Viewdraw Pin order file from this by deleting lines 1,2,3 and the last line(s).

*PADS-LIBRARY-PART-TYPES-V4*

00-441272 FPBGA224 I UND 0 0 0 224 0 224
A1 A2 A3 A4 A5 A6 A7 A8 A9 A10 A11 A12
A13 A14 A15 A16 A17 A18 B1 B2 B3 B4 B5 B6
B7 B8 B9 B10 B11 B12 B13 B14 B15 B16 B17 B18
C1 C2 C3 C4 C5 C6 C7 C8 C9 C10 C11 C12
C13 C14 C15 C16 C17 C18 D1 D2 D3 D4 D5 D6
D7 D8 D9 D10 D11 D12 D13 D14 D15 D16 D17 D18
E1 E2 E3 E4 E15 E16 E17 E18 F1 F2 F3 F4
F15 F16 F17 F18 G1 G2 G3 G4 G15 G16 G17 G18
H1 H2 H3 H4 H15 H16 H17 H18 J1 J2 J3 J4
J15 J16 J17 J18 K1 K2 K3 K4 K15 K16 K17 K18
L1 L2 L3 L4 L15 L16 L17 L18 M1 M2 M3 M4
M15 M16 M17 M18 N1 N2 N3 N4 N15 N16 N17 N18
P1 P2 P3 P4 P15 P16 P17 P18 R1 R2 R3 R4
R5 R6 R7 R8 R9 R10 R11 R12 R13 R14 R15 R16
R17 R18 T1 T2 T3 T4 T5 T6 T7 T8 T9 T10
T11 T12 T13 T14 T15 T16 T17 T18 U1 U2 U3 U4
U5 U6 U7 U8 U9 U10 U11 U12 U13 U14 U15 U16
U17 U18 V1 V2 V3 V4 V5 V6 V7 V8 V9 V10
V11 V12 V13 V14 V15 V16 V17 V18

*END*

[Carl_at_xrite]

Originally posted by Lameris
You can export the Parttype from PowerPCB and then use that to create a pin file as described from the Veiwdraw help below.

To create a pin order file:
1. Using any text editor, create a file using the .pin file extension in the sym
subdirectory.
2. List the pin labels in the appropriate pin order, separating the pin labels
with a space (or place them on separate lines).
3. Save and exit the file.

This is what the Exported Parttype file should look like from PowerPCB. Lines 4+ are decal pins 1,2,3,4,5 etc. It should be simple to create a Viewdraw Pin order file from this by deleting lines 1,2,3 and the last line(s).

*PADS-LIBRARY-PART-TYPES-V4*

00-441272 FPBGA224 I UND 0 0 0 224 0 224
A1 A2 A3 A4 A5 A6 A7 A8 A9 A10 A11 A12
A13 A14 A15 A16 A17 A18 B1 B2 B3 B4 B5 B6
B7 B8 B9 B10 B11 B12 B13 B14 B15 B16 B17 B18
C1 C2 C3 C4 C5 C6 C7 C8 C9 C10 C11 C12
C13 C14 C15 C16 C17 C18 D1 D2 D3 D4 D5 D6
D7 D8 D9 D10 D11 D12 D13 D14 D15 D16 D17 D18
E1 E2 E3 E4 E15 E16 E17 E18 F1 F2 F3 F4
F15 F16 F17 F18 G1 G2 G3 G4 G15 G16 G17 G18
H1 H2 H3 H4 H15 H16 H17 H18 J1 J2 J3 J4
J15 J16 J17 J18 K1 K2 K3 K4 K15 K16 K17 K18
L1 L2 L3 L4 L15 L16 L17 L18 M1 M2 M3 M4
M15 M16 M17 M18 N1 N2 N3 N4 N15 N16 N17 N18
P1 P2 P3 P4 P15 P16 P17 P18 R1 R2 R3 R4
R5 R6 R7 R8 R9 R10 R11 R12 R13 R14 R15 R16
R17 R18 T1 T2 T3 T4 T5 T6 T7 T8 T9 T10
T11 T12 T13 T14 T15 T16 T17 T18 U1 U2 U3 U4
U5 U6 U7 U8 U9 U10 U11 U12 U13 U14 U15 U16
U17 U18 V1 V2 V3 V4 V5 V6 V7 V8 V9 V10
V11 V12 V13 V14 V15 V16 V17 V18

*END*

Gary,
Thanks for the tip, I did find a better way to create the pin file.
I opened my symbol in the symbol wizard and selected all pins
I then used CTRL-C to copy the pin information and pasted it into Excel.
I then used the sort to put the pins in order and copied the pinname column into a text file..
worked great, no more problems.
Thanks again,
Carl