PCB Component Placement Webinar

Proper component placement is one of the most important aspects of PCB design. You need to familiarize yourself with the basic requirements for placing components on a printed circuit board and how they affect the other aspects of your design process (MCAD enclosures, production, signal integrity). Join us in this webinar as we explore the tools in Altium Designer designed to help you perform the perfect layout.

Learn how Altium Designer can simplify component placement while ensuring electrophysical parameters, mitigate mistakes, and speed up the overall electro-mechanical design process:

• Component Placement Requirements
• Mechanical Requirements
• Defining Keepout Zones
• Preliminary Components Placement
• Placement of components taking into account the Assembly Production, Signal Integrity, and Power Supply Requirements

Follow Altium on Twitter: https://twitter.com/altium 
Follow Altium on Linkedin: https://www.linkedin.com/company/altium/ 
Follow Altium on Facebook: https://www.facebook.com/AltiumOfficial/ 

Ready to try the industry's best in class design experience yourself? Download it today and get started! https://www.altium.com/downloads

Transcript

Nathaniel Pierce:

All right. Welcome everybody to placing components on PCBs in Altium Designer. This is intended to be about a one hour webinar. Depends how many questions come in. It's all about obviously placing footprints on your PCB. Okay. Now my name's Nathaniel Pierce. I've been working with Altium Designer since 2006. So I've done quite a few PCBs over the years, and here are some tips and tricks and the design process is what we're going to cover first. Okay. Before I get really too far into a demonstration using Altium Designer, I'm going to go through the majority of these slides. Occasionally I might interject what the slide show here to show you something in all teams.

But first thing we're going to review is the design process itself, right? So roughly here's the flow chart of the PCB design process, right? First in the upper left, right? You're going to create your schematics first, right? Then eventually you'll create a PCB file after you compile your schematics and resolve any errors or warnings, typically after you create your PCB file, the PCB doc, right? You'll import a board outline. Hopefully if it's been provided by your mechanical engineer or create the board shape yourself, if you can, there's a variety of ways to do that. Set up some design rules for component placement and routing and preliminary design rules are created before you even place any footprints on the board. And that's what we're going to focus on today of course, right? Then we create the board stack up. Hopefully that stack up is already created for you in a template PCB project, you would have a template PCB that's got a default layer stack up with about how many layers you'll think you need.

And once you have that board shape and your stack up, and some basic design rules defined, again, which is typically done in a PCB template project, then it's time to place your footprints, right? And that's what we're going to talk about today. And that's broken down into a couple different steps, some preliminary placing of components and then final placement as well. Okay? Because sometimes it's more important to place some footprints more than others. Okay? And eventually of course there are later steps in the design cycle for routing doing a final design rules check, preparing all of your output files, right? And then preparing those files for production for your bear board for fabrication and your assembly files. Okay? So typically we're going to have some placement required requirements for components. Okay?

Because we're going to have to be working with the mechanical engineer. You see this picture up here, right? Perfect example of where you have a product enclosure and there are going to be openings in the product enclosure, right? For switches, for connectors, for LEDs. So those components have to be placed very meticulously, very carefully in accordance with the openings in your product enclosure. And I'm going to show you a perfect example of that later on. Okay? Couple other things have to be considered as well, right? When you're placing these components, right? You've got to take into consideration all of the other components around them. Also, whether the board is going to have a rigid flex, is there a flexible section of the PCB where the footprints may interfere with each other depending on their height. Okay? So we've also got some other placement considerations for signal integrity, to avoid overshoot and undershoot and ring time like shown in this O scope of this signal down here at the bottom, right?

So we've got a lot of these considerations that we have to take into consideration, right? So again, we're going to discuss a little bit more taking a look here at these... The mechanical engineer requirements, because typically they'll have already decided what the board shape is going to be based on that product enclosure. Okay? So just read a question came in here. Again, just to let you know, I'm sure you guys probably have seen that there's a chat window and also a question and answer panel in the Zoom Webinar panel. Okay? All right. So it's up to you. However you want to ask any questions, you can type them into the question and answer panel or into the chat window. I'll see it either way. Okay? Now if we have to have a dialogue so that we get more information about your question, I can unmute any one of you at any time too. Okay?

So a question did come in here. What about that D1 section in this PCB, it looks like there's a board cut out there. How do I create a board cut out in Altium Designer? Good question. Okay. So what I'm going to do is I'm just going to open up Altium Designer briefly and show you. Here I've got to finish PCB, but I'm just going to create a new PCB with F for file N for new and P for PCB. You see that. So what that's going to do, it's going to create a blank PCB. That's R it's a template PCB that I've got set up in preferences. And watch this. If I open up the view configuration panel, look at this, it made a copy of my template PCB that I have, and it's already made a copy of all of these mechanical layers that I've specifically named with intuitive names to tell me the exact object set that's supposed to be placed upon them. Okay?

So again though, briefly, that's under preferences under the system branch under new document defaults. You see, anytime I create a new PCB and I've got a PCB project open, it's going to make a copy of this template PCB that I've got. Or if I don't have any PCB project at all, and I create a new PCB, right? That's going to be a free document. And that comes in here. It's using the same template PCB project. All right? So let me answer your question directly. How do I create a board cut out? All right. Look at this. I've already got a PCB here, just a four by six inch PCB. And I've got all the tracks and arcs. If I go to select all on layer, you see that all those tracks and arcs make up my board outline right there. But if I wanted to place a cutout, watch this, I'm just going to go to place, arc, full circle and draw the center of the circle and just move my cursor out so that it increases the radius and boom, there it is.

As soon as I right click to escape place full circle mode, all right. I escape that placement mode, but that object is selected. So then watch this. Here's the key. Tools, convert. You see that? Create Board Cutout from selected primitives. You see that option. Look at all of those options under the convert menu. I could make a two day class just from those convert menu options. All right. So right there, it instantly created a board cutout. If I go into 3D mode just by pressing the 3 key, and then I'm going to go to orthogonal rotation. In fact, you can see that board cut out. You see that? All right. And all I did was place a full circle down and then go to the menu bars. Tools, convert, create board cut out from selected objects. You see that's from selected primitives specifically. You see that. Now, hopefully that's already been done for you. Okay?

So check this out. I'm just going to close this PCB and not save any changes. And in fact, I'm just going to create a new one file, new PCB. All right. And in fact, what I'm going to do now, watch this. I'm going to select all those objects S for select Y all on layer. All right? And you see I've got nothing selected because I'm on the top layer. If I move down to the M1 PCB outline S for select Y all on layer, it's selects all the objects on that layer, bang. I just hit delete. All right? Because what I'm going to do is show you how to import a board outline that somebody else already made. All right? Now, I know that webinar is really more about placing footprints on the PCB, but you got to get that PCB shape first, right? So this will only take a second watch this. File, import, DXF, DWG. All right?

So I've happen to have a DXF file here. All right? So if this file import dialogue box comes up, look at this. I'm going to import it on M1 PCB outline. So now you see the value of me giving very intuitively named mechanical layer names. So as soon as I click, okay, that gets imported. You see that? And this is where that select all on layer command comes in very handy. All right? Now, under the edit menu, there are some other helpful commands for some of the more commonly performed features and options like edit, move selection. All right? I'm just going to put my cursor right here at an arbitrary place here. All right? And now, basically I could make my board outlined from this, but first, what I'm going to do is, you see to create a board outline Altium expects an enclosed shape, but it doesn't like those other objects that are there for cutouts.

You see this DXF file. It looks like this is a perfect example of a rigid flex PCB that's going to fold up. All right? But watch this. I'm just going to hit X for deselect touching rectangle and anything that's touching this rectangle or completely enclosed within it is instantly deselected. Again, I'm going to hit X touching line and draw a line between these objects to deselect them. And repetition is the mother of studies, right? So X for deselect, again, touching rectangle. And I'm just going to draw rectangle that touches those three arcs. And now with that enclosed shape, now, again, I can use this tool design board shape defined from selected objects. Boom, it's done. But you see this, the mechanical engineer included this section up here, look at this.

I'm just going to draw a box around this cutout area tools, convert. And once again, create board cutout from selected primitives. I'm just going to draw touching rectangle to touch that arc. Tools, convert, create board cut out from selected primitives. So you'll see that very often. You'll see that your mechanical engineer hopefully would give you that board shape. You see that, and that's the way to go. Okay? And now I'm just going to hit the zero key to set the zero axis VF to fit the board. And now I hit two to jump back into 2D mode. And of course, you'll see that in 2D mode, there are two different zoom settings. All right. So I'm sure that answered your question very thoroughly of how to create a board cutout. So now I'm going to close that PCB and not save any changes and let's get back into the slide show. Okay?

All right. So this is again, just revisiting this slide here that we saw about how the mechanical engineer is going to create that board shape for you with those cutouts. All right? And of course, we're going to have a precise location for some footprints in Altium Designer, and we would do that in the properties panel. You'll see, once you lock a footprint right there, the X, Y and location setting is deactivated. Okay. So that's where you would lock a footprint and enter the specific X, Y location for any of those footprints that you needed to have at specific X, Y locations, like a connector or an LED. Okay? So there are also some component alignment commands that we're going to take a look at a little bit later as well. Okay? All right. So let's take a look at the next slide. We're going to take a closer look at this and locking components and making specific footprint placement and aligning components a little bit later on. Okay?

Identifications of zones of prohibition on footprint placement and AD. All right. You can place what are called, keepouts. Okay? Good question. That comes in. How do I place a keepout? All right. I'll show you here in just a minute, but I just want to bring up a couple things in this slide, right? See what you can do. There's a bunch of placement design rules in any PCB. You open up design rules and go to the placement section, and you'll see that there are some generic footprint placement design rules that are created for you. Okay? And over here on the right they're showing that you can create a room, right? Just draw out a specific room out on a PCB. All right? And define a maximum height in that room. Okay?

So those are a couple things that we can do. And over here on the left, that's showing a screenshot from the properties panel, I believe when you place a specific keepout. Okay? So let me answer that question specifically, how do I place a keep out while I'm here on this slide? Why not? Okay? All right. So let's... Again, I'm just going to create a new PCB again. All right? And just a basic rectangular PCB here. You see it just added it to the existing project, but once I right click and close this document, if I don't save it with a name, that PCB is just going to be deleted as if it never existed. Okay? Now watch this though, over here in the view configuration panel, I'm going to pin this panel down here just for a moment by toggling on that pushpin icon. Okay?

So for example, you'll see down, the reason I pinned it down is I want to bring your attention in the layers and colors section here, down towards the bottom, under other layers. There's a keepout layer. And if you scroll down, you'll see, look. I'm going to make that the active layer. All right? Now I could have just clicked on the, keepout layer at the tab at the very bottom. Now, anything that you... When you... So to answer your question directly, how do I place a keepout? Well, if you want to make it a keepout on all electrical layers, select the keepout layer tab at the bottom of the main editing area and whatever objects you place upon it is going to act as a boundary that you can't place objects in. Watch this.

So if I go place, arc, full circle, and I just draw a full circle on that, keepout layer. All right? Down here. Let's just say, for example, and click to commit that radius right there. You see that? All right? Now, if I go back up to the top layer and I'm just going to click these arrows, click and hold that arrow and select the top layer. And now, for example, if I just wanted to route, Okay? On the top layer, look, I'm just going to go to the menu bar, PT place track. And look at this. As soon as I get close to that full circle on the keepout layer. Look at that. You'll see that it's obeying my clearance rule and it's not... It's only letting me get too close to that boundary right there.

And that's because I've got clearance boundaries enabled in preferences. You'll see under tools, preferences on the interactive routing page. You see I've got display clearance boundaries. It's pretty awesome. That's a really handy feature, I think. All right? So similarly, right? If I wanted to place a footprint down here, I'm just going to open up the components panel. I've gotten pop out mode over here on the right. You see this, I'm just going to place this random footprint down here. You see. And as soon as I get too close, if I go to put this bad boy down, look at that. There's that by default, that bright green color right there for a design rule violation. You see that?

Okay. So there are other ways actually to place keepouts as well. All right? So for example, all right? If I wanted to right on, I'm still on the top layer, right? Watch this. I'm just going to draw a box around everything and delete it. Watch this. Now what you can do is you can create layers specific, keepouts. Because earlier when I placed that circle on the keepout layer, that acts as a keepout for every routing layer and every plain layer. If I wanted to just place a layer specific, keepout for example, on the top layer. All right. Now I would say, "All right. Place, keep out." All right? So for example, in this case, right? I could say solid region. If I had a cutout or again, if I could use, use the full circle right here.

Now it's showing it as a layer specific keepout. And if I look in properties, look at that. It says, "Keepout arc." And this is where on that slide coming back, full circle to where a slide show, where we started. You see the keepout restrictions here, that section. All right. By default, it's keeping out all of these object types. You see that? So that if I go once again to place a track up down to that keepout arc right there. It's going to show that clearance boundary saying, "Sorry, you can't get in there." You see that? all right. So that's how you place a keepout. You can place it on the keepout layer or make layer specific, keepouts. In fact, another thing that you could do, if you wanted to, you could even place a room as a matter of fact.

You could create a room and place a room on a specific part of the PCB. You could go design, rooms, place rectangular room, for example, or any shape that you want. Watch this. So I'm just going to place this room right here. You see, by default, it just says room definition. You see that I could give it a name if I want to. And in fact, but you'll see that a room is actually part of design rules. You'll see that a room is down here and you'll see that. For example, it's just... But I just created it now called room definition. I'm just going to call that room Chip right there. Okay? That's my nickname by the way. And I hit enter, and look at this. I could say keep objects outside. You see that? Okay. All right.

Now look at this though. Instead it... By default it says false up here. I'm just going to say all. I just want to keep everything out of that room. All right? So here's just another way that you can do it. You see the room just inherited that name right there. And now if I went to place a footprint down in here and I go to place it in that room, it's going to bark at me right there. You see that? It saying, "Sorry, pal, you can't go in that room. You got to stay out." All right. And I've got online DRC enabled, all right? Which is doing live design rule checking. Okay? So those are some different ways that you can place keepouts very specifically on specific layers or for all electrical layers by placing objects on the keepout layer. Okay? And again, I'm just going to right click and close that PCB without saving any changes and let's get back into the slide show. Okay? All right.

So there are some design rules that we saw as well in here. I'll take a look at those a little bit later as well once I get into a full scale demo. All right? So if you'd want, you could do some preliminary placing of components on the PCB and that's very often going to... What you'll do is very often people will select a group of schematic components and enter what's called cross select modes that the corresponding footprints are selected in the PCB. And when you move one, you move them all. Okay? So in here, basically, they just showed a few preliminary component placement. And very often, you're going to have to add layers depending on how densely populated your board is. And remember component placement's very important because ultimately, all right? Your board, the routability of your PCB is going to be directly related to how well you place your footprints. And there's no substitute for experience here, folks. Okay?

All right. So there for the assembled board, right? There are going to be some notes and design rules that you create. So for example, in my PCB, in my template PCB, I've got all my mechanical layers named with very specific names for assembly notes, fabrication notes, dimensions. Okay? And we're going to take a look at that in a few minutes. All right? Now we have... There are some other parameters and things to take into consideration as well, right? How about some of these electrophysical parameters, for example. All right? If you have bypass caps that you're to an IC. All right? You want one connection and be as close as possible to the pad, right? And the other pad of a bypass cap typically is connected to ground, right? And that's going to be typically connected by pouring a polygon. Okay?

So again, you're going to have some specific requirements. I'd recommend that if you have specific assembly requirements for your PCB, of course, talk to your manufacturing engineer for fab and assembly. Okay? Because remember placing footprints on the PCB is really all about assembly. Okay? So for example, what they're showing you here is like an example of employing cross select mode and cross probe mode. These are a few tools naturally under the tools menu that can help you select the schematic component and the corresponding footprint is already selected. In fact, if you want a few components that you can select in the schematic, well, those footprints will be selected at once in cross select mode and you move one and you move them all. Okay? So this is how you go through it. I'll give you a demo here in just a moment. And there are some other on the PCB side, under tools, you'll see tools, component placement. There's a sub menu there that's got a variety of commands that can help you do a preliminary placement of your footprints. All right?

Okay. So here's a few different methods that they used here and a few different options in the schematic and PCB editor for selecting components. Okay? All right. So there's also another tool you can use is called unions. You can select a group of objects in the schematic or the PCB, right.

Click on it and say, add to a union. And then when you... For example, that's helpful for flipping a bunch of components to the bottom of the board. Okay? Now, typically that's done before you'd be routing, but if you wanted to, right? And you had some other connections that had to be made. If you knew you wanted to flip all of these to the bottom layer, you could do that very easily using these unions feature. Okay? Now I don't see too many other questions coming in yet. Okay? But I'll keep that in mind. And thanks again for your attention here. I'm just going to escape out of here and that's the end of the slideshow. So let's get into it. All right? Let's take a look and see what we've got here in this sample PCB I've got, you can see that there's a few blank sections of this PCB. All right?

But quickly, I'm going to take a look in the projects panel, because I want to bring something to your attention about this particular project. Okay? Now this particular project is a real Altium Designer product. All right? But it's created in Altium Designer. It's a USB JTAG adapter hardware device. That's intended to be used with a hardware tool called the NanoBoard that Altium invented some years ago. Okay? For hardware development. Okay. So it was originally called DT01 which means developer tool zero one. But I just renamed it, MY_DT01 because I made a few changes to this, just a few basic things. And I wanted to differentiate the original from my own. So you can see there's a blank section up here in the upper left and a blank section over here on the right where I basically have just removed a group of footprints.

But I wanted to use this example project as my demonstration here for you. Okay? Now what I did, there are 16 components here and this schematic, there are 16 corresponding footprints in the PCB that don't exist yet in this PCB over here, right? So typically whenever I'm in the PCB editor, I put my panels in pop out mode. So I'm going to do that in a minute here. But before I do take a look at the project structure here and you'll, you can see that this is a typical hierarchical project structure where I've got a top level schematic and each of the green sheet symbols represents subordinate underlying schematics, like this one that I've got open here. Okay? Now none of these corresponding footprints are on the board yet. So I could go to the menu bar, design, update PCB document, or from the PCB in this project, I could go design, import changes from my DT01.

And you see, it's going to add 16 components. It's going to add 19 pins to existing nets. It's going to add seven new nets. It's also going to add a component class and a room, which is by default created for every schematic in your project that has parts in it. All right? So I'm just going to click execute changes, all teams going to go through a couple of quick gyrations and I've always got to close the engineering change order dialogue box. Now there was a slight pause for a minute because online DRC kicked in. Now I'm in the PCB editor. So again, I usually put my panels and pop out mode to maximize the real estate in the main workspace over here. And look at this. If I zoom out, I can see here are my 16 footprints over here, off to the right. And I can see a design rule violation right away. You see R31. R31 is too close I suspect to the product enclosure.

Check this out in 3D. Oh yeah. It's showing that's a component clearance violation. I can tell for sure. All right? And it's intruding. It's colliding with the product enclosure there. You see that? So in 2D, you'll see when I zoom in, if I move this guy out just a little bit, okay. Now it's not complaining about that anymore because it's no longer touching. And you can see the component bodies. In fact Of the footprints that I just imported in here, you see that. Some of them are step models. All right? And some of them are just Altium Designer component bodies. Okay? All right. Back into 2D mode. A couple of things I'm going to show you here are some tips and tricks for component placement. But one of the things right off the bat, I'd know right away is that I've got a connector here. And this connector is going to be... It has to be placed at very critical locations. Okay?

So that it lines up properly with the opening of the product enclosure, this CN2. Remember that connector, I just showed you in 3D. All right. So assuming that you're working with your mechanical engineer and they gave you these X, Y locations, all right? This is where you would select that component and enter it in the X, Y fields up here. So I've got some coordinates here, 11462, 9697, and a specific rotation of 180. All right? And as soon as I hit enter bang, there it is. Okay? Now what I'm going to do here, let's take a look here is once I get that placed exactly where I want in here. Okay? I would lock it. You see that? So for example, back in the properties panel, boom, I click on that lock icon. You see that? All right. And as soon as I do that, all right? I can't move that anymore. Okay? All right. So again, what you can see in here, all right?

Is that you've got an option under preferences well, just to be checking as you're moving these components around. Okay? You can turn it on or turn it off if you like. I usually keep it on as I'm moving footprints, but because I've got that product enclosure in place, I'm going to see a lot of violations as I start moving components out towards the edge of the board. All right? So I'm just going to turn it off for now. Now a few things before I start placing footprints that I notice is that there are a lot of really big designators. All of these 16 footprints that came in have very large designators in comparison with the designators that are already on the board like this Y1. So I'm just going to select one of those designators that already exists on the board and examine it in the properties panel. And I see its height is 28 mills and it's width is three mills. All right?

That stroke width, three mills is pretty small. All right? So what I'm going to do, I'm just going to right. Click on one of these large designators I just brought in and select find similar objects. Now a text designator is just a text string, but what I'm going to qualify in the find similar objects is I want to specifically select designators on the top overlay that have a text height of 60 and a text width of 10, and I'm going to make sure all these boxes are checked at the bottom specifically this one that says, "Select matched," and click okay. All right. And now that opens up the properties panel where I can see at the bottom of the properties panel, 16 objects are selected, which is exactly what I wanted to see because I know that I just brought in 60 footprints. And I'm going to change the text height to 30 and the stroke width to five and hit enter and just click in the main editing area to deselect this designators that are still highlighted. So I'm going to right click and clear filter. All right?

So let's take a look at some of these helpful component placement tools. Okay? So back in the schematic, I'm going to show you how to what's called cross probe and use this cross select mode. You see that? All right. So for example, if I wanted to keep all of these parts up here near the top of the schematic, look, I'm just going to hit VD to fit the whole document and VF to fit all objects and pan down. Look at this back here in the properties panel with nothing selected. I'm going to turn everything off except components. And I'm going to go up to the menu bar under the tools menu and ensure that cross select mode is enabled. And you'll see there's a little blue rectangular box there. You see that? All right. So knowing that I have that cross select mode enabled and my pre selection filter is set to components only, boom, I just draw a box around this whole section of the top schematic and 10 schematic components are selected. Those corresponding 10 footprints and the PCB editor are automatically selected as well.

Okay. So now I'm going to zoom out, pan over to the right side of the board. You see, I've got them all selected. I'm going to go to the menu bar tools, component placement, reposition selected components. And one by one, they are all going to snap to my cursor and I'm just going to place them outside around the edge of the upper left section of the board, where I'm going to place all of these guys down. Okay? I'll just grab that guy right there. So that's preliminary placement just to get that group of components right over there. Right click in the main editing area in an open space, clear filter. Now, alternatively, what I could have done is cross probed, but you see you only cross probe one footprint at a time. Watch this. Tools, cross probe. My cursor turns to a cross hair and Ultium is prompting me at the bottom on the status bar it says, "Choose navigation point." You see that? So if I just click on this part, what it's going to do is quickly flash up the PCB and show that part.

But if I want to switch over to the PCB editor, I press control and then click on this IC6 and bang it selects IC6 and the PCB editor and zooms into it. And now I'm ready to place this guy. You see, when I move this footprint right here and now I hit the space bar to rotate it. And I'm just going to preliminary place it down there because guys what I'd recommend you place your larger footprints first. Right? Okay. So right click and clear filter. And then what I'm going to do is I'm going to use these connection lines as a guide. Now be careful though there's a zoom threshold. All right? For seeing the net names and the pad numbers on these pads as I get in a little bit closer. All right?

So for anybody out in the audience there taking notes, here's a really big tip and trick. Check this out. When you hit control, click, you'll highlight an entire net. Look at that. You see when I hit control click, it's just going to highlight the entire net and all of its connections like this one right here. So this is telling me right now, "Hey, put these footprints closer together." That's exactly what this intended function is. All right? So like L3, you see, as I go to move it's grabbing it right by the middle. It's grabbing it by its component reference point. And like IC6, I noticed that when I grabbed it grabbed it by pad 1. And generally speaking, that's not a good idea. Surface mount components, usually the component reference point is right in the middle. All right? Now watch this. I can turn on the component reference point.

You see it's invisible in view configuration. You see that? And for surface mount footprints, the component reference points typically in the middle, but someone made a mistake on IC6 and put it on pad 1. Typically, it's through whole footprints that have pad 1 as the component reference point, you see that? And I enabled that in the view configuration panel, underneath system colors. All right. So here's what I'm going to do. I'm using these connection lines as a guide and I can just... I'm clicking and holding and dragging and rotating as I go along. And I'm trying to avoid these crossover lines. You see that? On the bottom of L3 here, those lines are crossed over. So if I rotate it twice, they're nice straight lines. And very often I move my silk screen very often as I'm moving my footprints. Now, one thing I noticed here, that's a little odd, in the very lower left of my status bar.

I looked at my grid 0.004 mills. Now that's my snap grid. Now that's the original snap grid of this PCB. I'm not sure why they put it so low, but if you wanted to change the snap grid you could do it manually in the properties panel, underneath the grid manager, right? You'll see that they created it so small, right? You see that? I'm just going to hit the one key and just change the grid to one mill and hit enter. Now I won't see that one mill unless I zoom way in and then I'd see a zoom threshold there. Okay? All right. So let's see, I'm going to select that five volt net again, because what I'm doing is I'm grabbing these parts that are going to be located close to that. Now look the ground net, I'm not even worried about that ground connection because I'm going to be pouring a polygon over this top layer, ground net. And that's going to absorb These ground connection pads. So if I wanted to, I could completely turn that net off that ground net.

You see that it's not showing as a connection line until I actually move the part. You see that? And I've got another five volt connection for this guy right here. You see that? And now my large 90 degree cursor is actually helping me quite a bit to line up these different objects. You see, as I move this footprint, my large 90 degree cursor is helping me line up things properly. You see that? All right. That's up to you. There's a fine line between wasting time placing silk screen and doing a good job. Okay? So that's important. You see now that's going to be really easy to route. You see that? So I'm using these connection lines as a guide. You see how about VPP_ON. All right? There's one connection that's going way over it looks like this pad, all right? Knows the only connections there. All right? So it's all about zooming in and out.

And you can go look at these different components that are connected to different nets. These guys right here, for example, I'm just... I see these three guys are all going to be right around in here. All right? And this is just a little bit of preliminary component placement. You see that? All right. So let's take a look here. I've got... I can see this net VPP_ON maybe a little bit better if it would be even easier to route, if R42 was over here, watch this. You see, now if I bring R42 here and there, that's a shorter route. You see that? All right. So I'm just going to grab that guy right about there. And that five volt connection is still there. Let's do a little cleanup as I go along. Here's a couple of other connections in here. All right? Let's check this out. This guy right in here, for example. Okay?

Let's go here. And this guy... And let me just grab this designator and grab it over here. So again, using connection lines and rotating the footprints so that I can see where I've got a straight shot. You see that? And R45. All right? Is over here on the right. Let's take a look here. I'm going to just grab this guy and rotate it a few times. Now, there's another cool command I can use. Watch this. Under edit, move, move. You see that? Move, move. Now I can just click once. I don't have to click and hold and drag. Shift and space bar is going to rotate it clockwise for me. And again, I'm not too concerned about that ground connection, because as long as I have enough room for it to connect to a polygon, I should be in good shape. And again, I'm going to line up my designators over here on the right over here. I've got a few other connections.

How about D4 let's take a look at this guy right over here. All right? So let's see. This is connected to 12 volts and this connection right here looks like it would work very nicely. Okay. That could work or I could just do it this way. I suppose if I wanted to. That would work. That's going to work real nicely actually right there and select D4. Every... I use this PCB occasionally for my Essentials class. I teach the Essentials class and I always try to mix up the footprint placement just a little bit on here. Okay? All right. So let's take a look here. What else I've got here? I've got a few other footprints that are close to the edge of the outside the board. I'm just going to drag them on for the time being and take a look at their connections. All right.

This is 12 volt and ground here. All right? So C5. And 12 volt and ground over here. You see that? All right. So what I can do here, I can just grab this guy over here. I've got plenty of room. All right. I'm going to put all the designators then on this side for these guys. And again, I got to be careful that I don't waste too much time with the designators, right? You can lose your mind with that after a while. All right? So I can just put this guy right here. I got a straight shot. And this is also 12 volt and ground, right? You see that? I'm using my right mouse button to pan over here. All right? So that looks pretty good. It'd be pretty easy to route that. All right? So watch this. Here's a few different commands as well I can use.

First, I'm going to clear filter. And let's see. I'm going to draw a box, select touching rectangle. Just select those three parts right there and go to the menu bar, edit, align. Check this out. All right? Align horizontal centers. You see that? Now my cursor's going to turn to a crosshair. And along the bottom on the status bar, it says select a primitive because it wants me to choose one of the footprints to use as a reference to where it's going to move the other ones and line it up with it perfectly. And it just shifted R40 and R45 over just a little bit. Now I'm going to hit A for align again. It's got its own shortcut keys, right? Now, I'm going to say distribute vertically. You see that? So that the space between all of them is equal and it just moved R40 a hair. I'm going to select up C15 and R42. You see that?

And let's take a look here, edit again, align. And let's see how about align vertical centers again? You see that? And it just wants me to choose a reference. I'll grab R42 and it shifts C42. I can grab these guys here as well. Okay? And let's take a look here and see what some of the aligned commands I could use here. Again, I'm going to use that align horizontal centers and choose F5 right there. And it's shifted FC4 over. Okay? In fact, you could really experiment with this quite a bit. Here's another align command. Okay? And let's see, how about align vertical centers. All right? And use this one. So now they line this guy up. All right? And if I wanted to, again, I could use that A for align, align vertical centers for those two and use R40 as a unit right there as a reference.

All right. So you can use some of these align commands. So now I've just got a straight shot for a lot of these routes here. You see that? All right. Now, basically, I could see if I wanted to run a design rule check on component placement there. All right? But that falls out of the scope of this webinar just a bit. It's all about placing components here. Okay? So that you use the connection lines as a guide. And I can see, I don't have any crossovers except one for this net here called VPP_ON. And it's going way over on the other side of the PCB. So I would expect that I'm going to probably have to drop a VR2 to make that connection eventually, unless I wanted to do some rerouting and get some of these traces out of the way there.

All right. So I'm going to just going to write click and clear filter VF, view fit board. And of course you can see I've got some other footprints off to the side here and I'd use those same placement techniques. All right? Rotating the components properly to straighten out those connection lines. And that's what it's all about folks. Placing components on the PCB. You can use some of these commands, like cross probe and cross select mode. All right? Which I leave enabled all the time, cross select mode's really helpful. So we've got some of these semi automated tools to reposition the selected components as well. All right? So for example, if you wanted to, for example, for unions. All right? A question came in about, how do I create a union? All right. So if I wanted to keep these parts together, right? Watch this, I think I still have my selection filter, just set to select parts.

All right? So for example, if I... Yeah, I do. All right? So I could check that out in properties, but I just drew a box around all these five parts, right? Now, if I wanted to right here in the schematic at that point, man, I could just go right click unions, create union from selected objects. You see that? And it tells me five objects added to a union. I click, okay. I'm going to click in an empty area, the main editing area to deselect that. And now on any one of these parts, I can just right click and say, "Unions, select all in union." They're all selected over here on the PCB as well. All right? Now, if I wanted to, I could even route these connections first, but now that they're all selected, right? Over here in the properties panel, bang, I could flip them all to the bottom layer, just like that. You see that? All right.

So that's what the properties panel is all about. Okay. Another question came in, where did the silk screen go? Good question. Okay. The silk screen went to the bottom overlay layer, but here's the deal. The reason you can't see it, look at this. The bottom overlay is turned off. If I turn that back on now you'll see all. That everything that was on the top overlay layer flips to the bottom. And that's what they mean here when it says, "Component layer pairs." See, when you're making this footprint, right? You're going to... Whatever objects you put on top overlay, you flip that part. It goes right to bottom overlay, right? That's how you... That has to do with layer pairs. Okay? All right. I'm going to click once in the main editing area control Z is your friend. All right? And now I'm going to hide that bottom overlay layer, right? At the bottom of the main editing area. I see it's layer tab. I'm just going to right click on it hide bottom overlay and right click again clear filter, shortcut key shift C shift Charlie over. End of demo.

If there are any other questions, I'll wait for a few moments here and examine the question and answer window and the chat window as well. But I'd sure like to thank everybody for all your attention to this webinar. And I'll stick around for a few more final questions in here. Okay? All right. So I'm just going to let some of the... First thing I'm going to do here that... Though before I start answering some of these last questions, what I want to do is ask you guys a few poll questions in here. Okay? So if you could answer this question, please, and I'll give you a minute to answer, I've got three different questions that I'm going to ask to for you guys. Okay? So let's take a look here. I'm just going to allow you guys to vote and allow you to continue there. And in about another minute, I've got three questions here for you guys. And once I... After a minute or so, I'll move it on to the next question. Okay?

All right. And it looks like all of the attendees have answered that first poll question. So I'm going to end that and launch polling again, but this time I'm going to ask a different question. Okay? Hold on here just a second here. Let me just close this out. I've got to select the second polling question. Pardon me there just for a moment here. And here's a question in front and the second polling question, if you need to create a group of components directly in the schematic, is that necessary? Okay. And I see that all of our answers have come in and let me ask the third question in here about footprint placement.

Okay. And that this question again has to do with preliminary footprint placement. So it's a good idea, yes, to prearrange those components. All right. Well, that's the end of the polling. I could share the results in here for everybody as well. And there you have it. Okay. And here are some of these final questions in there. Let me share these results as well. It looks like... Okay. Okay. Let me stop sharing those results then. And those are these different questions that we have in here. Okay? Well, that's all I've got for you. I appreciate your time, everybody. Again, my name's Nathaniel Pierce. It's been a pleasure to conduct this webinar for you. I teach the essentials class, which I'd highly recommend. If you have not experienced the Altium Designer essentials three day training class, I would highly recommend that you contact your account manager and try to enroll. Now you can go to altium.com and you can see under training event and events when that comes up next. In my default web browser here, I'll just show you real briefly here under resources, training and events.

Now, in this case here, I'm just going to filter down to show the Americas and to show you that you can create, see that in English. The next Essentials online trainings is on May 5th, looks like there's still room, and you could also do this training class on demand. If you just wanted the training materials, you'll see that you can scroll down and see that that training class is on demand and you can buy instant access to those training materials for a 1000. It's 2000 for the online live training. And if you wanted to take the online classroom training, that's $2,500 face to face training. Okay? So again, that's altium.com resources where you can see training and events, webinars, technical papers, video library. All right?

So there's a lot of resources here to help you get up and running with Altium Designer. And once again, thanks again for attending this webinar. And if you need to get any of that training, feel free to contact your account manager and they'll set you right up. All right. I'm going to stop sharing now and stand by for any final questions. Once again, thanks again for attending this webinar. And I look forward to seeing you hopefully at the next Altium event soon.