Dokumentieren für Fertigung und Bestückung mit Altium Designer und Draftsman – AltiumLive 2022

Alexsander Tamari
|  Erstellt: Februar 3, 2022  |  Aktualisiert am: Juli 1, 2024

In dieser Sitzung werden die Funktionen von Draftsman in Altium Designer mit Vorlagen und benutzerdefinierten Dokumenten ausführlich behandelt. Außerdem schauen wir uns die wichtigsten Elemente an, die Ihr Hersteller, Bestücker oder Fertigungsunternehmen in diesen Zeichnungen sehen möchte.


  • Demonstration des Draftsman-Tools in Altium zur Dokumentation für Herstellung und Bestückung
  • Wie Sie Vorlagen in Altium definieren
  • Demonstration der Erstellung einer Fertigungszeichnung in Altium
  • Wie und warum man das Tool „Feature Control Frame“ verwenden sollte
  • Wie Sie Ihre Designs im Altium-365-Arbeitsbereich teilen können

Zusätzliche Ressourcen:


Alexander Tamari:

Hello everyone. My name is Alexander Tamari and I'm a technical marketing engineer here at Altium. Today, I'll be talking about documenting for fabrication and assembly using Draftsman. This presentation is going to be mainly focused on the Draftsman tool within Altium Designer. So let's get started. On the agenda for today, we'll talk briefly about what fabrication and assembly drawings are, why you need them and what they should include. So first let's talk about the what and the why. So what are, and why do we have fabrication and assembly drawings? Well, fabrication and assembly drawings are additional notes and diagrams included with your final design package that you hand off to your manufacturer. And what they do, they give a deeper insight and clarity to your manufacturer for how you want your board to be made and assembled. Let's first talk about the fabrication drawing. Now, the fabrication drawing specifies how the physical board should be made, and it will include things like the drill table, drill drawing, layer stack up, a dimension board, notes and possibly more depending on what and how you want to convey your information.

The assembly drawing on the other hand, that mentions the details about how each and every component will be attached to that board. And it will include assembly notes, any special instructions or requirements and component outlines and the board outline. Now these drawings are needed. If you only provide a Gerber file, the manufacturer may miss out on the additional details concerned with the board. So really if you want to get your board done right the first time you should include these fabrication and assembly drawings as part of your manufacturing package.

I mean, no one wants to get a phone call in the middle of the night or emails back and forth of their manufacturer just asking for more information, things that you could have and should have made clear before you sent out your final package, documentation package. So one thing I would also recommend is speak to your contract manufacturer early on, not just when you're doing your documentation. They can help you very early on in the stage, even when you're just defining your layer stack. Actually, this is something I have heard a few times recently, which is not being able to get the board materials. I mean, we're all hearing now about electronic part shortages, but there's also shortages and delay from getting board materials. So maybe if you speak to your manufacturer ahead of time and they could tell you, "Hey, we don't have this material. Here is an alternative that you can use."

Just to save yourself time later on that way you don't have to go through the whole scramble of using this new material. Maybe you have to redesign depending on the specs of that material and go through the whole approval process. Just do it, save yourself a whole lot of trouble later on. Anyways, let's move on. So what should you include? Some of the things that you should include with your drawings. Well, there's a few things, of course, every drawing is different, but there are some things that you should include when creating them. First, let's talk about the fabrication drawing. The fabrication drawing should include a note section, which gives specific instructions to the fabricator that really can't be included elsewhere. And this could be something like asking the fabricator to comply with a specific standard or anything else that really wouldn't be part of your Gerbers.

You want to include the stack up, which shows the number of layers as well as the materials and thicknesses, board dimensions, drill table, and drill drawing. As for the assembly drawing, you'll want to include a note section. And this is going to be similar to the fabrication notes except geared more towards assembly. So if you have any special instructions or requirements, you'll want to add them there. You also want to include the board outline and component outlines as part of the drawing, and you should include your bill of materials. And it's also so nice to have some additional views and perspectives of how your board should look or your final board should look.

So how was this done before Draftsman? Or maybe you're not using Draftsman or even Altium Designer. How things were traditionally done is with several different programs. So in days past when making these drawings for your documentation, you'd have to import and export between several tools to create these drawings. So you would need maybe a 2D drawing tool or an MCAD tool for the dimensioning of your board, maybe a Word to build a custom table or a bill of materials. There are also third party all in one tools, something like Blueprint, which you can import your design into and create these drawings. But really the problem with all these tools, using all these different programs or using a third party all in one program is that it isn't synced with your design. It's a disjoint process.

It's not synced with your design. So when a change is made, because changes are always made, when a change is made to your design, you're going to have to import and export between each one of these programs. And that's not, I guess it, I was going to say, it's not necessarily difficult. I mean, it can be a real pain in the butt to redimension, redraw, fill out new tables because those aren't really automated, it's all kind of a manual process. And it's all that importing and exporting with all these different tools. You could be, you're just opening yourself up to a higher chance of error. So I've been speaking to some manufacturers and fabricators and one of the biggest mistakes, or maybe it was the biggest mistake that they keep seeing with their drawings is that the revisions, or the drawing doesn't match their design.

There's always a discrepancy because changes are made, but they're not updated in the documentation. So how do you solve this? Well, you do that by using Draftsman. Draftsman, which is part of Altium Designer, really has everything you need to create these fabrication and assembly drawings. And the best part is it is synced with your project. It's part of the Altium Designer unified design environment. So if you make a change to your design, that change is reflected in Draftsman. So you're always sending out the most up to date information. Also it's free and it's part of Altium Designer so there's nothing extra you need to purchase or install.

So now let's go into Altium Designer and take a little tour of Draftsman. And we can see how it works, we can also see how easy it is to create these fabrication and assembly drawings. So let's get into it. I'm going to just move over to Altium Designer. And here we are in Altium Designer. We have my board here in 3D. Here it is in 2D. And actually this is, this board has a variant, and you can see really the difference between the variant and, well, okay, the variant is the Note:FPGA Ram variant. That's what we have it named here. And it's really just removing the memory and some capacitors and these two LEDs here. So you could see those have been removed from my variant.

So what we want to do is create a fabrication and assembly drawing for this PCB. We want to templatize it so we can share it with the rest of our team via the Altium 365 Workspace. That way someone else later on, on another project who wants to import your template and they could start using, or they can start creating their fabrication assembly drawings, not from scratch, but from what you've already put into it. So let's get started. We want to create a new, oops, a new Draftsman document. Now just looking right here in this menu, we have different templates that we can choose from. We have templates on our local machine here and also on Altium 365.

We can see those are here and it's signified by this cloud. What we will do is just choose default because we want to have a blank canvas to work on. And first thing I want to show is the Properties panel and the Document Options. So make sure you have the Properties panel open, you can open that by going to panels properties. And just like you would in any other editing environment, whether it's the schematic or the PCB environment, you always want to have the Properties panel open because the Properties panel is your informational hub. It's where you can customize and view information about what you have selected. And in this case, since we have nothing selected, we are being shown document options. And there's three tabs here, there's the General tab, Parameters and Page Options. Under General, we can mess around with the grid sizing, color, snapping options, how we want variants to be displayed, documents, blinds, colors, patterns, everything that has to do with this document and appearance.

Under the Parameters tab, we see all our parameters, our system parameters, schematic parameters, PCB parameters. Actually wait, is this schematic? If I hover over this is going to be can be system, PCB and project, it wasn't schematic. I know I messed up on that, project, system and PCB parameters. And lastly, the Page Options tab we can choose, or we can define the document itself. So we can define its width and height. We can choose from a standard height or a standard document dimension, and also choose a template. And these templates can be pulled from my local machine or my workspace. Again, signified by the cloud here and the computer screen here for the local. Before we move on, let me just show how I'm zooming in and zooming out. It is the same as the other editors. So control, scroll for zooming in and out. I actually use the mouse wheel button to zoom in and out. So control, scroll to zoom in and out. Shift, scroll to go left and right. Right click and drag is to pin.

And I believe that's it. Okay. So what we're going to do is build our own template. We're not going to use the template here. Let's just choose, I guess it really doesn't matter. We'll choose this document size and we're going to create our own template. And to do that, we're going to use the place panel, place panel, sorry, the place menu. The place menu can be located up here or by pressing the P key on your keyboard. Now, when you're in Draftsman, the Properties panel and the place menu are your two biggest items you're going to be looking at. So I would just use the keyboard.

I think it's a little easier, but of course you can do whatever you feel is best. So I'm going to go ahead and choose the line tool. And I'm just going to start to draw. Trying to go quickly because this isn't really the most exciting part of the demo. So maybe my lines, oh, I mean they're pretty straight, it snaps to where it needs to snap. Okay. So here I have the beginnings of my title block. I want to go ahead and place a graphic here. And here I have the Altium Designer logo. Of course, I can adjust the size of that and next I'm going to place some text and the parameters.

And actually what I can do here, let me change the color of these lines from black, sorry, from purple to black and make them a little thicker just so I can see it better. Oops. I missed this one. And let me place some more text here and we can call this title. And so what I want is this to be called title and then this to be the title of my project, of my PCB. So I'm going to click this button here to add a parameter and then I could just choose a parameter from my list here. So I'm just going to choose that there. Oh, that was leftover, that will be that title.

This one can be, let's call it rev, let's choose the revision here. There you go, PCB rev A, not a new text, don't need that. And you know what? Let's say we have a company part number, but we don't have that parameter in our parameters list. We can always add it. And the way we will add a parameter is by right clicking on our project in the projects panel, going to the project options, parameters, and we could add a new one. We can call it company part number and we'll give it a value of 12345. Press okay.

And if we type equals company part number, it will be populated. And you'll notice as I move this around, this text box around, it's snapping into alignment in regards to the other text boxes around it. And this allows you to keep things nice and straight in straight columns and rows. And that helps with the readability of your document later on. And it's just, it's a little nicer on the eyes. So there we have it. This is our template. I don't remember if I've mentioned it, but there are two types of templates. There are document templates, which is what we saw when we created a new Draftsman document. These are document templates. There's also a sheet template that applies to a specific sheet, and that's what these templates here are. What we're going to do, we're going to save this as a sheet template. So to do that, we'll just go to file save as, and from the pull down, we'll select Altium Draftsman sheet template and we'll call it sheet template demo.

Great. So now this is saved on my local machine, but it's not available to everyone on my team. To make it available to everyone on my team, I want to share it to my Altium 365 Workspace. And to do that, I'll go open the Explorers panel. And in my Explorer panel, it's taking a look at my workspace. And in my workspace, I've defined a section for Draftsman templates. I have document templates and sheet templates. What I'll want to do is create a new item here and I will create a new Draftsman sheet template. I'll call this sheet template demo and before I press okay, I want to make sure that this is checked off. And what that will do is, well, let me tell you what having it checked on will do. So if I press okay while this is checked on, a new Draftsman document will be opened within Altium Designer so I can start to create and edit my sheet template from scratch. But since I've already created this template, I just need to upload, I don't need to make a new one. I'll keep this checked off.

So let me press, okay. And now, right click and press upload to upload the document on my local machine onto my workspace. So now it is uploaded for my whole team to use. But to be honest, this doesn't really look nice. I'm going to go ahead and delete it and then for the rest of the demo, we'll use the default template. Okay, great. So now we have my template of my nice title block pulling information from my project. And now let's start to build out this fabrication drawing. So this fabrication drawing, I want a layer stack legend. I want a board outline that I can start dimensioning and a note section as well as a drill drawing, drill table and layer views for each one of my layers on my board. So let's get started. First, I'm going to press P and start to place the, excuse me, layer stack legend.

Now this layer stack legend, it's grabbing information directly from the Layer Stack Manager within Altium Designer. So this is all exactly what I have in my design. This is actually a little bit too big. So in the Properties panel, I can go ahead and adjust the look and feel. So I can adjust blinds, text, all that stuff. I'm just going to change the display mode to the default. And I will place this up here and now let me start placing some views here. I'm going to place, I want an outline of my board that I can dimension.

So let me go ahead and place that view. I'll place it here. And I could adjust the sizing. I can just drag the corner, make it bigger or smaller. I could use a custom scale or choose a scale from the pull down and custom scale. So if I say 1.56, it'll make it 1.56 to one, but let's just have a scale of one to one. I'll place it here. This is my fabrication drawing, I don't really have a need to see these components. I really just want to see the holes and the board outline. So what I'm going to do is turn off the visibility of those components.

I'll show all my components, control A, to select all. Disable those views and press okay. So now I have my board with the holes and you could adjust the view settings for your hole. So let's say, in this case, I just have holes, sorry, I'm getting tongue tied in my own head. I will only be able to see holes of 1.5 millimeter or greater in this case. I want another view. So I'm actually just going to do control C, control V. And you'll notice that these are snapping into place. It may be kind of hard to see. I'm not sure how great it looks on your end, but on my end, I see two blue lines, one at the top, one at the bottom and a green line in the middle.

That's just letting me know that I have aligned these two designs or these two views together. And again, it's just like with the text, things are aligned, it looks clean and it's more readable. I'm going to change the view from top to a right side view. So I'll go ahead and place that here. And now I can start to really dimension my board, but before I dimension my board, I want to define my date in planes. So again, place, and I'm just going to go ahead and put these in.

So I have my plane, A, B and C. So let me put those in here. This I will label C, this B and I can keep the other one as A. Cool. So with that defined, actually let's put a center mark, because these are pretty cool. So these just snap to the center of my holes here, you could see, just snaps right to the center. Okay, let's go ahead and start dimensioning. So these are my dimensioning options. I have the linear. So if I click on a straight edge of my board, it'll dimension that. I could also the distance between two lines, two sides.

Radial for my curved edges, diametral for my different hole sizes. I have angular, so this will be the angle between two sides. And in this case, this is 90 degrees. Nope, ignore that. Let's do that one more time. There we go, and let's do ordinate. First you choose the reference, which is here and now these will just snap to the center. And these are all the dimensions as referenced to the origin here. Move that closer. There we go. And actually let's just place one more linear dimension for this thing right here.

One more thing. I do you want to add, if it gets enough love, which is the feature control frame. So I can place that and let's do it to this hole here. I could adjust that. So let's say I want to adjust this for the position, I could do that here. Let's do the tolerance of 0.2 and as reference to A and B. Cool. There's one more thing I want to add on this page and that is the notes section. So let's go ahead and do that. And again, notes section here you can place maybe if you want adhere to specific standards. So let's actually go ahead and do that. I could just type that in here.

Maybe this one I could do RoHS-Compliant. So I say, all materials shall be compliant. I don't know, this one could be a flammability, I don't know, whatever you want it. Any other standard has to adhere to some sort of flammability rating that can be in here as well. So we have our notes, we have our layer stack legend. We have our dimensioned board. Now what we want to add is the drill drawing and drill table. There's really not enough room here. So let's go ahead and add a new sheet. Again, use the place menu and add, where is, here we go, a drill drawing view. It's a little too small for me. I'll add a drill table.

And this drill table can be customized here so I can turn on and off different columns to include whatever you want. You could even break this up so you can have a drill table just for blind vias, drill table for through-hole vias or anything else. So if you want to make those specifications, you really want to show that off. Actually, I don't think in this design I have any impedance controlled lines, but you could also place a transmission line table. Yeah, you can place that here as well.

Cool. So I think that's it for the fabrication drawing. Let's go ahead and, actually, nope. I knew I was missing something. Let's add a new sheet. I want to add some fabrication views for each one of these layers, each one of the layers on my board. So I'm going to the go ahead and place a fabrication view. I'll change the scale to 2x so we can see it a little bit better. I'll copy and paste that right here. So this is my top layer and on the right hand side, I'll have my ground layer. And I'm going to go ahead and do this for each one of my layers.

So mid layer one and then mid layer two. And I'm not going to bore you with it, but I would go through each one of these layers and place that view. It's the same process. So now I have my fabrication drawing and what I want to do is just like I did with the sheet template, save this as a document template. So same process. I'm going to file save as from the dropdown, select Document Template and I'll change the name to document template demo. Now when I press save, I get this little warning. It's more of a confirmation as the box says, and this is just letting me know that dimensions, callout, sectional views, detailed views, these views that are specific to a project will not be saved.

Just as an example, dimensions, those are not going to be saved as in the template because they will not apply to another design. So those will disappear. So I'll press okay, those have gone. And now this is saved as a document template on my local machine. If I want to share this with everyone else in my team, I'll have to put it on my Altium 365 Workspace. Again, same process. Let's go ahead and create a new Draftsman document template item, and we'll call it document template demo. For the same reasons as before, since I already have this document existing, I don't need to create one so I'll check that off. Press okay. And now I can upload that document.

Great. So now this document template is shareable and accessible to everyone on my team. So we've got the fabrication drawing done. Let's move on over to the assembly drawing. I'll go to file new Draftsman document. And you'll notice that that document template demo that we just created is available for us to use. We don't need it at this moment. So let's go ahead and create a blank drawing. Again, we have our blank canvas. Let's go ahead and use that same template.

And now we can start to build out our assembly drawing. What we'll want to show is different board views with the components and component outlines, as well as some, maybe an isometric view to show more detail of how the board should look. Oh, actually, we could add a realistic view and a bill of materials, we'll add those. So let's get started. First let me place my views. So I will place a board assembly view. And again, Altium Designer is pulling all that information, all that component information, board information, and it builds this view out.

Actually, you know what? Let me go ahead and delete this and go to the document options. What I want to do, since we have a variant, let's go ahead and use it. I want the source document to be the variant. So now when I go ahead and place my assembly view, it's going to pull information from the variant document. So you'll notice that these components are in red because these are non fitted components. So I'm going to go ahead, copy and paste this. I'm going to have a few views here. This is going to be a view from the left side. This is going to remain the top side. This will be the front.

And you notice again that it is snapping into place. And this is also going to be the top view, but we just want to show the silkscreen. Cool. So now I have my different views. Again, I could select and move them wherever I want. I want to show off some things. I want to have some callouts. I want to use the board detail view. So if I zoom in here, I can see in detail, but maybe when I print this out, or if someone prints this out, it's not as easily noticeable. Or if I want to highlight something, I can go in here and use the board detail view.

And I can change the scaling of this. Maybe I want this three to one so I could really get a good look. I'll have these connected. And instead of saying detail A, let's say these are my test points. Let's go ahead and add some notes so I have something I can call out to. And let me just start typing in some notes. So I can say spec to IPC 610. Maybe here I will put interface test systems.

And let me add one more note. So I'll press the Add button here, new one appears, and I will call or have this note be a non fitted components. So how do I associate this non fitted components with these red mesh pattern components? I'll actually just use a rectangle in this case. So let me just add a little rectangle here, select it and I'll change the pattern. That way I know whenever I'm looking at this pattern, these are non fitted components and this also works in black and white as well. I kind of want to change this note here to have a square. This doesn't need a square.

Okay. So now I want to call out to notes item two and three. So let me go ahead and do that. Under annotations, I have a callout and I can select this component here. Change the source text to a note item and choose note item two. Let me go ahead and place another rectangle here, because I know I want my certification stamp to be right here. Just change that to black and have this filled in. Great. So now let's place another callout and do the same thing except associate this with note item number three.

And again, with all these views, with these callouts, the notes, you can adjust the text, the colors, how it looks, the line with. So everything is all here in the properties panel. I did want to add a board isometric view. I know I mentioned that, and that's just going to give me a more, kind of like a 3D view of the board, more at an angle like a 45 degree angle where these top side view, left side, front side view is more looking at it from a 90 degree angle or a normal angle. This is going to be at 45 degrees. So let's go ahead and change the face side to front, because I think that looks better.

So it's just rendering that image right now. There we go. And let's make this a little bit bigger so we can see it. There we go. This is dumb, but it's bothering me that it's 1.56 so let's just make it 1.5, an even 1.5. There we go. Great. And just to point out, I don't know if I did, but this is all, this template is pulling information from the board. The variant, it has the Note:FPGA Ram variant name here. And I know I mentioned this in the slides, but I haven't shown it here yet up until now. And that is, one of the great benefits of having Draftsman is that it is synced with your project. It's part of the unified design environment. So if a change is made to your design, that change is reflected in Draftsman.

And, gosh, I can't remember if I mentioned this in the slide. So I want to mention it one more time. I'm sorry if you're hearing this for a second time, but the biggest discrepancy or the biggest problem these fabricators or contract manufacturers have is getting a board or getting documentation with a different, sorry, getting documentation that is different than the design. The revision of the document let's say is 32, while your design is on 33, that discrepancy is very common and Draftsman will solve this problem. So let's go ahead and make a change to my board. What I want to do is actually just get rid of these capacitors here. I'm just going to delete them just so it's an easy visual comparison. So let's go in this design.

I selected these in 3D. They're also selected in 2D. We'll just delete them and you could see they are gone. So what I'll do, I'll go back to my document and if I right click, I can import the changes. So right now Draftsman is going to go into my Layer Stack Manager, my 2D PCB layout, my 3D drawing, it's going to pull all that information, component information and it's going to update every design, the isometric views, the assembly views, of different angles. And you notice they're gone here and they're gone from this view.

I actually want to put those back. So I'll just control Z, put those back in my design and again, import the changes. So we'll be able to see that it appears here in the front view, the isometric view, top views, everywhere. There we go, and they are back. Okay. So we have these views here. We have our notes, our callouts. Now what else we need for the assembly view is a bill of materials. So let's go ahead and add a new sheet and add a bill of materials. There you go, and we can just place it. Again, we can adjust the fonts, colors. We could go over here to the columns tab of the Properties panel while having the BOM selected and turn on and off different columns. So we can really customize this however we want. So if I want to add a manufacturer, boom, it's right here.

Also, oftentimes when you have a bill of materials, it is a very long, and it might not fit on one page. So if you want to break up your bill of materials, you can also do that here. So if we go here to limit page height we can, right now the max page height is 200 millimeters. So let's say we changed that to 100. You notice that it went from one page to three. So let's go ahead and name this bill of materials. If Caps Lock's on, that's okay. I'm going to copy and paste. Again, it snaps into place.

I'll call this not page one, but page two and then select page two from the pull down. And again, you could do the same thing for the third page. Same idea. Now let's go ahead and finish up, add some different views. We'll add the complimentary views to these. So this is the left top and front. So we'll do the right bottom and back views. So let's go ahead and place these assembly views. So I will copy, paste. This is going to be, actually we'll have the right there, it's okay. Right, bottom silkscreen, and this is going to be the back. So let's ahead and change this to back. This is going to be right bottom and then this is going to be my bottom silkscreen.

Cool. There we go. Let's just align this a little nicer. Yeah, that's good enough. Okay. So we have all that. There are some more views I want to show. I think since we do have a little bit more time, might as well go through it. In the place menu, there is something called the board realistic view. This is kind of a cool view. Let's make it a little bit bigger. So this is just pulling from my PCB data, my 3D environment, and I can customize it. So let's say I have a very specific view I want to show, maybe, I don't know. This specific view is really what I want to show so I can have this image in my documentation.

So I'll go here, I'll click the custom radio button for view and take a current camera position. So now it gives me the same view I have in my 3D environment. And if I want to match the colors in this case, it's a blue board, instead of green, I can take the current view configuration and it will adjust the view settings for me. So I could have it exactly how I have in my 3D layout. So if I really want to show something very specific, I can do that. Cool. And again, we won't go through saving this as a template, but you can save this organization to use.

And actually, let's do this. And let's use the document template. So if we click on the document template demo, the one we just created, press okay, this is what it's going to do. It's going to go into your design. It's going to take in all the views that we had. So we placed the layer stack legend, we placed notes, the assembly view. And what else was there? The drill table, drill drawing. It's going to place all that in here so we don't have to. So we can just pretend that this is a different design and it will recreate all of this information very quickly. So we have our notes, layer stack, the different layers, the fabrication view of my different layers, drill drawing, drill table. So very quickly you can build out this documentation, make a change, right click and import the changes if you make any changes.

So it is a very powerful tool. Also, you can include this in your document output. So if you have a, I think it's somewhere, an output job file. So if we double click on this output job file, let's open it up. We can include my Draftsman documents here. And then you could package it up, send it to your manufacturer via the Altium 365 Workspace. You can share it with them directly there. Or if you like maybe more traditional methods, you can do emails. I like the workspace because it's under version control. You can see everything that happens. It's managed and you can see the design in the workspace. So they can actually comment in the design.

How much time do we have? Do we have, let me just check. I think we have some time. I wasn't planning on this, but let's see if I have something up. So let me go into workspace and see, actually here it is, I haven't touched this design in a while, but this is my design in the workspace. So if you share this with your manufacturer, they can actually go in, see the design, leave different comments. They can search for components, see the schematic, the PCB layout in 2D. They can adjust their view to show different layers, the 3D view. And of course, you can move all this. So this is movable. You can click and interact with it. So you can see the details of these components. Of course, when you share with your manufacturer, you can limit exactly what they see, you can limit what they can and cannot see so you're not giving away your IP.

Let's go back here. I think this one might have a, oops, a release history. I'm not sure, but here, okay. We have some sort of release package here. And so you can see the different files included in this package. And this is under version control and yeah, you can send this to your manufacturer here just by sending their email and then specify what you want them to see and they can have access. It's very cool. So let's go back here. I think we're done. We went over creating a fabrication and assembly drawing, the different views involved, how to customize those views. Templatizing it so you can share it with your entire design team. So if you guys have any questions, I can answer those. I'll do my best. I was supposed to click the slide where we have 12 Draftsman. So thank you very much. And I'll be here to answer your questions. Thanks.

Über den Autor / über die Autorin

Über den Autor / über die Autorin

Alexsander kam als Technical Marketing Engineer zu Altium und bringt jahrelange Erfahrung als Ingenieur in das Team ein. Seine Leidenschaft für Elektronikdesign kombiniert mit seiner praktischen Geschäftserfahrung bietet dem Marketingteam von Altium eine einzigartige Perspektive. Alexsander schloss sein Studium an einer der 20 besten Universitäten der Welt an der UCSD ab, wo er einen Bachelor-Abschluss in Elektrotechnik erwarb.

Ähnliche Resourcen

Zur Startseite
Thank you, you are now subscribed to updates.