Designing PCB in Ultiboard

After you have finished and tested your circuit design in Multisim, it is ready for Ultiboard.

1. Transferring to Ultiboard

In Multisim, select Transfer »Transfer to Ultiboard
The save prompt dialog should open and point to the same location as your Multisim circuit is. Save it according to what version you’re working on. In case you need to return to a past design.
If you have virtual components, like Ground, it will tell you that your virtual elements will not be exported, click OK.
Ultiboard starts automatically and a dialog asks if you with to accept the Default Track Width and Clearance. 10.00 or 20.00 mil is recommended for the default Trace width. To be cautious and avoid traces cross talking, choose 20.00 mil for the clearances. Later, you can change the individual trace width if needed. Click OK.
The next dialog is the Forward Annotation Action Selection, it displays the components and the nets that will be transferred into Ultiboard.
You can Exit Multisim once the transfer is complete if you want

2. Board Outline

You can edit the size and orientation of the Board Outline to suit your needs. In the Design Toolbox click Board Outline. This allows you to edit items on a particular layer.
Select or delete the Yellow rectangle. You can then change the size or you can draw a new outline depending on your casing. Drawing is quite similar to Multisim.
Also, if you need to add holes for screws, you can add those too. We will discuss this further later to match the holes with the drill bits we have for the milling machine.

3. Layout of Your Design

A good idea to do before laying out the board is to draw out the major and critical components on paper. This will help you determine the overall orientation of the design.
We used to prefer single sided boards. The reason was our old way of creating PCB’s was a very delicate process. It was fairly difficult to create a complex single sided board. Creating a complex double sided board was not enjoyable. Making sure all of the drill holes were perfectly lined up and the traces didn’t wash away. Wasted multiple boards.
Now, it doesn’t matter. It’s just as easy to create a double sided board as a single.
In the Design Toolbox, unclick the Copper Inner 1 and Copper Inner 2. This only leaves Copper Top and Copper Bottom. 2 Layers.
Grouping similar components is an easy way to lower noise and power losses.
1. Place individual systems in separate locations on the board.
2. Separate sensitive components away from “noisy” components. Keep analog away from power supplies.
3. Separate components with different frequencies. Analog and Digital.
4. The same goes for different input/output components. Analog and Digital.
5. Different problems that systems can have: Grouping Components
Use Ground planes instead of intertwining traces. However, don’t place a component smack in the middle of one. Try to create one in a large open section of your board.
Ground traces should be as short and thick as possible.
Major Power traces can be thick if possible, but not as necessary as Grounds.
Ground and Power planes and traces should be in close proximity to each other if possible, don’t send them in opposite directions around the board. This lowers loop inductance of your power system.

4. Editing Individual Component Pads

Make sure your component pads and your actual components in your hand are the same size. Print out a 1:1 ratio of the component and stick it through the paper to be sure.
If it’s not, click on the component, then select Edit » In-Place Part Edit. This allows you to select the individual pieces of the component. Move or edit the pads or whatever to where they need to be. Unselect Edit » In-Place Part Edit when done.
You can also go Tools » Component Wizard and create a component.

5. Traces – Make them look GOOD

If you want to try the Autoroute, go for it. Then you can adjust the traces if you don’t like them.
Double click on the Copper layer in the Design Toolbox you want to place the traces in.
Then select Place » Line and draw your connections to your components.
1. Try to keep the distance as short as possible. The longer your traces are the greater it’s resistance, capacitance and inductance.
2. Traces should only have angles 45 degrees. Try to avoid right angles and under no circumstances use an angle greater than 90 degrees. This is important to give a professional and neat appearance to your board. That’s really the only major reason for this.
3. Forget nice rounded trace corners, they are harder and slower to place and have no real advantage.
4. Make sure the traces go through the exact center of the pads and components. Again, looks and gives you the most clearance.
5. “Neck down: between pads where possible. Changing your trace from large to small and then back to large again if you need to go between pads.
If you Power and Ground traces are critical, then lay them down first.
Symmetry is very professional. It’s all about the looks.
Don’t place vias under components.
Try to use through hole components to connect top tracks to bottom tracks. This cuts down the number of vias needed. Less holes, less time to assemble.

Examples of GOOD ROUTING (Left) and BAD ROUTING (Right)

6. Creating multiple power planes

If your design requires separate power/ground planes, use the next steps:

Go to Place->Shapes-> Rectangle (or polygon), specify its size/location/layer,
Select shape, go to Design->Convert Shape to Area,
Select created area, go to Parameters, specify the Net to which it must be connected, and connection style.
For the last power plane you can simply use Power Plane command, that will add plane to the entire PCB.

7. Finishing

Review all of the traces and connections. Make any changes that may need it.
Is there anything that could be done better?

8. Exporting

Select File »Export
Select Gerber RS-274X
Click Properties
Select from Available Layers:
- Copper Top,
- Copper Bottom,
- Board Outline (Optional)
- Drill-----The available sizes of the drill bits we have in stock (mm): 0.5,0.6,0.8,0.9,1.0,1.1,1.2,1.4 1.5,1.8,2.0,2.95 & 3.0.Please make sure your drill hole size is available.Otherwise change the hole size according to the availability.
Move them to Export Layers. Click OK.
then Export.
Create aperture mapping - Copper Top. This is the details of the components in each layer. Click OK.
Save export file. The file name should be already be something like:
- BCI(Example) - Copper Top.gbr
Save each of the files as they are listed.