Component Patterns

April 14 2016

The schematic is nearly finished. I still need to sort out how I will handle power selection -- probably just with header pins for the first version. I double-checked the BOM spreadsheet, making sure every component had a PartID.

I need to make sure every part has a land pattern before I can begin laying out the board. This is another tedious task. It isn't difficult and each individual part doesn't take more than a few minutes, but it is extremely detail-oriented and easy to make mistakes. This is also where I refine the BOM and update the project library components to include the information for exactly the part that is being used. When I am done, all the components used in the schematic should reference only the project-specific library.

The part name in the BOM should be a combination of the DipTrace component name and the Autotronik name. For example:
MSP430F5529-LQFP80 TPD2E-SOT553
The first part of the name lets me quickly find the component in DipTrace. The second part lets me quickly find the component in the Autotronik PnP component library. The two names are not equivalent! The PnP machine only cares about the shape of the component, all LQFP80 components are the same, all 0402 resistors use the same component definition. DipTrace needs to know the exact component, including its pin assignments and values.

The most methodical approach is to start with the BOM parts list. For each PartID:

1. Find the first RefDes. For example, PartID 1 is U201.
2. Go to the schematic and look up the component name by its RefDes. U201 is "LQFP80 - MSP430F5529".
3. Go to the component editor, make sure the project library (CtrlMtr01) is selected, and select the component "MSP430F5529".
4. Click on "Pattern" in the properties and verify the correct land pattern is shown.
5. If there is no pattern or it is the wrong pattern, I need to create the pattern and assign it to the component.

To create a new pattern:

1. Open the pattern editor and make sure the project library is selected.
2. If this is a standard pattern such as 0402 or 0603 I can copy the pattern from the stock library.
3. To create a new pattern, I first need to look up the pattern in the component datasheet.

   The easiest way to do this is to look up the part by its VendorID (from the BOM) and then enter the VendorID on the vendor's website (Digikey). The component info should include a link to the manufacturer's datasheet. For complicated components like an MSP430, I need to be careful to pay attention to the full part name. In this case I need the land pattern for the MSP430F5529IPNR. For example:
   U201 > PartID 1 > Vendor=Digikey/296-27306-1-ND

   

   The LQFP-80 is a 14x14mm die with a 0.5mm pin pitch. This is the stock DipTrace pattern "QFP-80/14x14x0.5". I measure the pattern to make sure the pads are slightly larger than the pins. I copy the pattern to the project library, rename it LQFP-80 to match the name of the MSP430 part, and save the CtrlMtr01 library (not the standard pattern library). Now I can go back to the MSP430F5529 component's attached pattern window, click on the CtrlMtr01 pattern library to refresh, and select the "LQFP-80" pattern. The pins should magically attach themselves. Verify in the datasheet that pin 1 is actually P6.4.

   

   
   
   

   I forgot to apply custom paste shrink to the pads, and the first build resulted in far too much solder and catastrophic bridging. Every pad should have a paste shrink value, with large pads having significant shrink values. See .

   
   

   Create an additional field named "Library" and set it to the pattern library name. This will be very helpful when copying the pattern into other libraries later.

   Click OK to save the pattern, then save the component library. Go to the schematic editor, right-click the component and select "Update from library..." > "Similar Name Components". Now I should be able to right-click the component, select "Properties" > "Attached Pattern..." and see the new pattern.

   NOTE: Updating the component will lose any changes made to that particular instance of the component, such as which pin names are shown. Don't bother setting the pin visibility until the schematic and component selection is final.

Updating a pattern for an existing component:

1. Update and save the revised pattern in the pattern library.
2. Open the component library, select the component, click Pattern... and select the new pattern from the library. This needs to be done even if the referenced pattern is the same; the component library keeps an internal copy of the pattern that needs to be updated. Save the component library.
3. Open the schematic, select an instance of the component, and select "Update from library... Similar named components". Save the schematic.
4. Open the layout, renew from the related schematic.
5. Select an instance of the component in the layout and select "Update from library... Similar named component". This extra step is necessary to update the shrink/swell attributes.
6. Export the TopMask, TopPaste, and Top gerbers.
7. Launch GerberLogix and load the gerbers, then verify that the pattern changes are present.

I found an error: I had Q204,Q101 marked as a 6MHz crystal (Digikey 490-1204-1-ND) when the LaunchPad uses 4MHz (Murata CSTCR4M00G15L99, Digikey 490-7861-1-ND). Then I have Q401 as 4MHz when it should be 6MHz.

{THREAD_LINK:1434} I need to double-check that pin 1 and pad 1 are properly connected; the datasheet for the fixture doesn't concern itself with actual pin assignments.

=====

April 15 2016

22:00> The component patterns are complete, time to begin the initial layout!

22:40> Premature declaration of victory... All the caps were symbols without patterns. I had to create components for polarized and non-polarized 0402, 0603, and 1206 caps and then replace all the components with the new ones. I need to verify the cap sizes.

I am still missing one pattern for the switches. I plan to just use header pins and jumpers, so I need to replace the switch components with 2-pin headers.

May 25 2016

The first layout used too much solder paste and failed due to bridging and pieces that floated onto a single pad. I applied paste shrink to all the patterns in the project to reduce the amount of paste applied to the pads. The holes for the header posts were reduced from 0.040" to 0.035".

The revised CtrlMtr02 layout with minimal paste areas:

My concern now is that the paste area may be too small to catch the components during placement, especially the 0603 and 0805 caps and resistors.

Once I have a working build, I need to migrate all the components and patterns from the CtrlMtr libraries into the EZ430 libraries to use for all future projects, then down into the CANMtr libraries.