In this example, we will be looking at building a circuit in Eagle and exporting it to Workshop for simulation.

The first step is to make sure that you have already unzipped the Eagle libraries and the ULP needed to convert Eagle schematics to Workshop into the appropriate Eagle subdirectories. The zip file should have been installed with B2 Spice A/D v4 in the same directory and is named "". Unzip the ULP file to Eagle's ULP directory and the *.lbr files the Eagle's LBR directory.

Start Eagle and bring up a new schematic. You will need to place the following items:

- 8 resistors from the RCL library. You can either use the US or EU symbols and any package, depending on your needs. For this example, the R-US R0603 was used.
- 2 capacitors from the RCL library. You can use either the US or EU symbols and any package, depending on your needs. For this example, the C-US025-024x044 part was used.
- 9 grounds from the supply1 library
- 4 OPAMP_IDEALs from our bb_parts_nopkgs_OpAmp library.
- 4 VOLTMETER2s from the bb_parts_nopkgs_Analog_Meters library.
- 1 VOLTAGE_SOURCE from the bb_parts_nopkgs_Sources library.

Place the parts so that they are roughly in the following positions. You might need to rotate some parts to get them in the right orientation. The OPAMP_IDEALs will first have to be mirrored and then rotated into the correct position. The schematic so far should look something like this:

At this point, it bears noting that some parts were used from Beige Bag's libraries (bb_parts_*.lbr) and some parts were used from Eagle's own libraries. The parts pulled from the Beige Bag libraries will correspond with a part in Workshop so they will import with a simulation model and will be included any simulation. As a rule, most parts from Eagle's libraries will not have a Beige Bag equivalent, meaning that those parts will not simulate. They will still be imported into Workshop but will be symbol-only parts and will not be included in the simulation. However, standard parts like resistors, capacitors, inductors, ground, and certain other parts that we've mapped into Beige Bag parts will automatically have their equivalent Beige Bag parts insterted and will have simulation capabilities. For a full list of the mapped parts, run Beige Bag's Database Editor and go to the "Edit->Edit Eagle-B2 Spice part and pin maps" menu. You can also add more mappings here if you find a good match between your Eagle parts and Beige Bag parts.

The next step to take is to wire the schematic. Wire the schematic so it will look like the following picture:

You will now add values to the devices. Assign all the resistors with a value of 10K. Both capacitors will have a value of 0.0159u.You will not need to assign values to the OPAMPS, VOLTMETER2s, and VOLTAGE_SOURCE. The OPAMPS are subcircuits and have all their values assigned inside the subcircuit. The VOLTMETERS2's are just meters and need no value assigned. The VOLTAGE_SOURCE will have to be assigned in Workshop as there are more values than can be assigned in Eagle.

You can just as easily skip this part and assign values after importing it into Workshop. But in this case, we'll assign the values in Eagle and have them exported to Workshop automatically.

After assigning the values, save the schematic and you're ready to export the schematic to B2 Spice.

To export to B2 Spice, click on the "ULP" button or File->Run... in Eagle and select the ULP "bbSpice.ULP". If it's not there, make sure that you have unzipped the ULP from the zip file that was installed in the B2 Spice A/D directory. See the note in the second paragraph for more details.

Once the ULP is finished running, look in Eagle's main directory for the file that was created. It should be named the same name as the schematic that you saved, with a .BDF extension. For example, if your schematic was saved as "new_schematic.sch", the ULP output will be called "new_schematic.BDF". If you didn't save your schematic before running the ULP, look for "untitled.BDF".

Run B2 Spice A/D v4 and go to the "File->Eagle->Create Circuit from Eagle file". A dialog box will pop up asking you to locate the BDF file that was created by the ULP. Select it and Workshop will start the process of importing the Eagle schematic. During this process, Workshop will import each part, seeking part matches in its database. If it finds a match, the part will be inserted automatically. If not matching part is found, only the symbol will be imported. These parts will not have any part in any simulations you run and wil be displayed in RED. Hopefully, all the parts will come in without problems.

The first thing to do is to check over the parts and wiring to make sure that all looks right. If a part is displaying in red, it means that a matching simulating part in Workshop could not be found. This circuit should not have that problem as long as you're using the latest versions of Eagle and Workshop.

The next thing to do is to set up the components so that they are ready for simulations. The capacitors and resistors should already have their values assigned from Eagle. You will then need to set up the values of the voltage source. To do so, double click on it and you will be presented with the following dialog box.

In the DC Value box, type in 5 for the value. Then click on the "small signal AC and Distortion" tab at the top of the dialog box. There you will find AC parameters that you'll need to set. The dialog box should look like the following:

In the AC properties area, type in a Magnitude of 1. Make sure to check the "Use" checkbox.

OK the dialog box to accept changes.

The OPAMPS need no changing as they're subcircuit parts pre-set with the parameters need for simulations. You can right-click on them and select "Edit simulation model" to examine the subcircuits.

The VOLTMETERS also need no changing as they're just probes that will show up as signals in the graph after you run the simulation. You can change their names to something meaningful if you wish. Double click on the voltmeters to set their names.

Now all that remains is to set up a simulation and run it. Go to the "Simulations->Set Up Simulations" to select the type of simulation and its parameters. You should see a dialog box like the one below:

Place a check next to the AC (AC Frequency Sweep) box to enable AC simulation and then click on the box itself to set up the AC simulation properties. You should see a dialog box like the one below:

in the "Start Value" box, type in 100. In the "Stop Value" box, type in 10K. In the "Number of Steps per Interval" box, type in 100. Leave the rest as is.

Click OK to accept everything and get back to the circuit page. Click the green double arrows in the toolbar to start the simulation. The resulting graph should look like the following:

Notice that the signals on the graph correspond to the voltmeters placed in the circuit. You can still add other signals by choosing the node to plot, or even making your own custom plot with the built in functions.

This should give you a quick tour of the process of building a schematic in Eagle and bringing it in to Workshop for simulation.