Hello Welcome back. In this video I'm going to show you how to transfer your schematic you created and capture cis light to a PCB and PCB editor light. So, how capture C is open with your project available to you and click the project tab over here it's named led dot OBJ. Next, you want to expand these folders here, this is the design file. And this is the schematic page. They want to rename this so just right click the schematic folder and choose rename.

You're gonna change the name to led ch or schematic and hit enter on a keyboard. Next, you want to change this page name. So right click it and rename it to the same thing as your folder here, led SC H, hit enter. What I'm going to do is duplicate this circuit onto a new schematic so that I can leave the simulation alone here and just create a new scope. That what I would use for mechanical purposes because he'll have to make some modifications to it. So, back in the project tab here, right click on the design file, then choose New schematic.

Let's name it led PCB, and hit enter. Now right click the LED ch schematic file and choose Copy. Right click this new folder led PCB, choose Paste. Now expand this folder and notice that the LED schematic page has been duplicated on to this new folder. So that's good. Go back to the project tab.

And let's rename it because it can get a little confusing when you have a lot of schematic pages. So right click and choose to rename the schematic page. We'll name it led PCB net okay. All right, last thing that needs to be done is I'm going to close these pages. So right click and close them. Okay, you want to right click this LED PCB folder and then choose make route.

This will be the focus of our PCB. So double click on led PCB now and we're going to work with this circuit to greet the printed circuit board and PCB editor light. So first things first, you need to delete this V DC here. This is just for simulation purposes, you actually need real connectors to connect to the schematic. So click drag and highlight this along with the wires, hit Delete on your keyboard and then that disappears. Next thing you need is to add a connector.

So in the place part option if you don't know how to get here, just let me show I'm going to close this window. Alright, so if you don't know how to get to the place part option, just click on Place part or tech p on your keyboard. Alright, so we're going to add a connector. Now I know the library components from memory and I've done so many designs in the software I know it's named c o n one, but it doesn't show up. Whenever this happens, it doesn't show up you need to know the library for the part is available. So click on the Add library button.

Now by default I'm in the P spice folder. I'm going to click the drop down menu here. And let's go to the cadence 17.2 folder under their tools capture library. I'm going to go one above the P spice folder. The connector I'm looking for is in the connector dot o lb libraries. I'm going to click on it and choose Oh Barry shows up on the connector con one not visible.

So double click on con one and place it right onto the circuit here. Make sure this red dot shows up as a caution symbol here, but don't worry about that click and place it. Place the other one here, right click and choose Add mode. Now we have physical connectors that connect to your PCB. Next, what we need to do just go to File, Save, make sure that's in good order there. Now click drag and hold and select all these components.

Go to Edit Properties. Make sure in the lower left you have the parts tab selected here. Also click drag and hold or click hold and drag to the right so you can see the reference numbers for your components. Lastly, let's drag this bar here to the right. Until we see PCB footprint, this column. Now there's already a footprint name as associated with the resistor, I'm just going to go ahead and delete that.

So click it, hit Delete on the keyboard, you're going to use some PCB footprint names that are already in the standard libraries when you install the software. So for resistor, type in rs 400 for the connectors, we'll use jumper one. Not for the LED, I found a pretty complicated name for the footprint for this part. So I put a notepad here. And it's a really long name, just feel free to pause the video. So you can type this in or save it somewhere.

Alright, so with this footprint name, just double click and right click, I'm going to copy it, put it right in the PCB footprint field for the diode. I hit Ctrl V on your keyboard to paste it and there you go. Right click this tab here and choose Save so that the schematic is saved properly. Now go back to your schematic tab and all your parts have a footprint associated with it. Next thing you want to do is go to the project tab and make sure led PCB is still your root folder. Click on the LED PCB schematic, choose tools, create netlist and we're going to transfer the schematic to a printed circuit board.

So choose Create eight or update PCB editor board not net ref. And just before we do this, I'm going to show you how to set up your PCB editor environment and PCB editor light. So go to your Windows start menu. All Programs cadence release 17.2. I have a lot of folders here you may not see as an under the orchid like product. Choose PCB editor like, I'm going to enter light mode.

Okay. Now how do you set up a new PCB? Well just go to File, New. Choose the board wizard, and then name it led PCB. Click the Browse button. I'm going to place this PCB inside the project folder that I'm working in right now.

So go to libraries documents. I'm just going to navigate to the LED folder. I'm going to make a new folder, too. So let's, let's name it. Allegro, all lowercase. Enter on your keyboard.

Go into the Allegro folder and select open. Now click OK. And the wizard starts. So just keep clicking Next, until you get to the option where it asks you about let's see here. The spacing constraints Set the minimum line width to 20 mils or 20 thousandths of an inch. The default via patch stack, you have to select one here, so click on the ellipses and then type in via hit tab on your keyboard. I'll go with the V 26 actually, click OK. And then hit next.

Now I want a rectangular board so I'm going to choose that. click Next again. The 1000 mil width and height here is more than enough space for what I need. So I'm just going to stick with that and choose Next and Finish. Alright, so the outline of your printed circuit board has been made. In the next video I'll show you how to continue this PCB design process in PCB editor light