What's with All the Layers in Your PCB Footprint?
Вставка
- Опубліковано 24 чер 2024
- Tech Consultant Zach Peterson responds to a viewer question regarding footprint layers. These layers correspond to PCB layout layers that designers work with in their PCB editor. So the question is, which of these layers are absolutely necessary, which ones do you need to create in pairs, etc? Zach dives into these areas and more in this PCB design video.
0:00 Intro
0:35 Essential PCB Footprint Layers
4:19 PCB Footprint Example
11:27 Keepout Layers
14:05 Assembly Drawings
16:15 Essential Exports
For more Component Creation videos, click here: • Component Creation
For more PCB Design for Beginners videos, click here: • PCB Design for Beginners
For more Tech Consultant Zach Peterson videos, click here: • Technical Consultant Z...
👉 What's With All the Layers in PCB Footprints?: resources.altium.com/p/whats-...
👉 4 Steps on How to Create a Component Footprint in Altium Designer: resources.altium.com/p/how-us...
👉 Working with IPC Compliant Footprint Models: resources.altium.com/p/workin...
👉 Original Question from Your BGA and You: • Your BGA and You | PCB...
👉 15 Days Free Altium Designer Access: altium.com/yt/altium-academy
Don't forget to follow us on social to stay up-to-date on the latest Altium Academy content.
👉 Follow Altium on Twitter: / altium
👉 Follow Altium on Linkedin: / altium
👉 Follow Altium on Facebook: / altiumofficial
👉 Ready to try the industry's best-in-class design experience yourself? Download it today and get started! www.altium.com/downloads?utm_...
The Altium Academy is an online experience created to bring modern education to PCB Designers and Engineers all across the world. Here you can access a vast library of free training and educational content covering everything from basic design to advanced principles and step-by-step walkthroughs. Join industry legends as they share their career knowledge, review real-life design projects, or learn how to leverage one of Altium's leading design tools. No matter your level of experience, the Altium Academy can help you become a better Designer and Engineer!
About Altium LLC
Altium LLC (ASX:ALU), a global software company based in San Diego, California, is accelerating the pace of innovation through electronics. From individual inventors to multinational corporations, more PCB designers and engineers choose Altium software to design and realize electronics-based products.
#Altium #PCBdesign #ElectronicsDesign - Наука та технологія
You should create a video on the topic of fudicials as well.
Thanks for cool supporting to all Altium team !! Very interesting and informative. Convenient for understanding. As soon as possible give us new classes. We will wait new your videos.
Zach I was looking forward to this video but was a bit disappointed - probably too much to cover in a short video. Not enough information on paste masks or linking the component layers to the PCB layers and please don't ask your fabricator to sort out your design otherwise you will need a new fabricator pretty soon! Looking forward to part II:-)
hi sir,ur videos are very informative,i want to know how to make slots for clearance in high voltage boards,plz make a video on slot holes sir.
Thanks, this video was in reponse to my comment.
It must be realized that all those extra layers like 3D Body, Assembly, Courtyard e.t.c need to be created as layer pairs. This means that they will not be created as Mechanical Layers but as component layer pairs. In this case we will add information onto one in the pair (probably the top) and leave the other layer in the pair as blank. Now, when a person uses this component in a PCB and they flip the component so it is used on bottom side, since we used layer pairs, everything on top portion of the pair will goto the bottom (automatically) and everything on bottom will come to the top. This power is only obtained when we use layer pairs. If we do not use pairs and just create mechanical layers for 3D body and other stuff, then when the use the component on bottom side, all those markings will still stay on the top side.
There is one more layer created by Altium wizards called "component center". What benefit does this have for the user or the fabrication or assembly house? I mean I do not see the benefit of defining where the component center is.
Actually the assembly etc do not need to be created as pairs unless there is suff on the opposite layer that requires assembly information. For the 3D body, you might have a mechanical model spanning across 2 layers, so it's not like you are creating a layer pair. You could set the standoff height so that the model passes through the PCB and appears on the top and bottom simultaneously.
Also the component center layer is not required, many people do not use it. The 2D centroid information already gets exported from the CAD data when you create pick-and-place file so you don't need to also create a component center layer, that center layer is for the designer's reference.
@@Zachariah-Peterson How is the component center layer actually used by the people that need it?
@@user-ww2lc1yo9c I think it would be to see exactly where the part will be grabbed with a pick-and-place machine in order to check that the placement will not be blocked by something.
@@user-ww2lc1yo9c I personally use it for manual (visual) component alignment and as reference points for snapping. Quite practical both with relatively big area components and even small ones like caps and resistors.
I like the concept of the component layer pairs and actively use it, but find it frustrating that IPC wizard has the only option to generate single mechanical layers. As a workaround I do the following trick: I generate the footprint by IPC wizard and load the template of mechanical layer set with a minimum component layer pairs predefined like 3D Body, Assembly, Courtyard and Designator (mech layer numbers corresponds to the default provided by the IPC wizard). This automatically places mechanical layers content on the corresponding component layer pairs.
Unfortunately, one can not store mechanical layer set in the cloud workspace, export/import is possible only on the local disk (yet another strange implementation in Altium).
Thank you. But I hide all the labels, contours and names of my parts. My boards always come clean with parts only. No names or shapes printed. High end suppliers' boards are like that. 😊
Hi Zack. Two questions please if you have time.
1. Right now I've got my footprint design convention to placing assembly outline, .designator, and 3D body all on the Assembly Layer Pair. Is there a downside to doing this? Otherwise stated, using this convention, could I still differentiate within Draftsman and Gerbers which individual types of primitives to apply for a given output generation? If not, I will change my assignments to give each one their own layer.
2. Regarding adding layer "text" to all layers such that they are printed into the gerbers to clarify what is gerber layer is for PCB fab... it seems like this technique would generate DRCs, is that true. For example, placing Copper text on Top Copper that is outside the board outline would most certainly generate a DRC I would think. I presume one would then attach a "No DRC" to the text to avoid the error? If so, could you please explain how to do that? I know how to do it in the SCH, but not how to do it in the PCB.
1. Based on what you write there is no downside to doing this, assembly outline and designator are standard in the assembly layer, and the 3D body once placed will be in its own 3D body layer. For the assembly views, draftsman applies the view automatically, so there is no need to manually differentiate. Fabrication view allows you to select which layers are prioritized along with a copper layer, so you have some customization.
2. You will generate DRC errors if placed into copper layers or silkscreen, solder mask, or paste layers and there is overlap with some other element that violates clearance. You can place whatever you want in mechanical layers, assembly layers, and courtyard layers and there will not be any DRC error, even if you have collisions. The reason is that these other layers are used to create drawings, they are not used in fabrication so the fabrication process will never see these layers.
@@Zachariah-Peterson thank you!
Is there a Altium Design Standard which Mechanical Layer should be used for what function? I see in the that M1 is used for the 3D model, which were previously added to M13 together with the component outline.
From what I know, there is no standard. However, there is an important point. You see when you create layer pairs, you can specify what kind of data the layer pair represnets. It could be something like 3D body, assembly e.t.c. Now if you have different PCB libraries with different symbols using different layer numbers, from I know it should all work out at the end since Altium designer can work out what layer pair contains what information.
Yes there is no specific standard, both in the industry and in CAD tools. Each CAD application has its own approach to using these mechanical layers. But you can name them whatever you want. For example with board shape, Altium has a board shape layer that it auto-generates when you export Gerbers, you can see it when you configure fabrication outputs. However you can create your own board shape layer as a mechanical if you want, and you can select this layer to be exported as the board shape.
Recent versions allow you to specify a "purpose" from a drop-down list for mechanical layers. This was necessitated when they moved from 32 mech layers to unlimited. Previously you just had to make sure your libraries and boards had matching layers arrangements, with this new approach the e.g. "courtyard" layer from the library will map to the "courtyard" layer in your board.
@@Zachariah-Peterson One thing I am looking forward to on the internet is detailed use of Altium Designer with HyperLynx for high speed PCB design.
@@Zachariah-Peterson I saw your video on solder bridge jumper. I have a few questions. The component is called solder bridge jumper. It is not called 0R resistor jumper. I guess this means that we should just put a bit of solder on this component to make the connection and then later we can just desolder it to remove the connection. Isn't that the basic idea that we only need solder to make the connection and not a 0R resistor? This point has not been discussed in the video at all.
Thank You. I am having a different requirement. I have to make a PCB footprint of a patch antenna with slots and an internal coupler which are spanned in different copper layers (3 copper layers to be specific). How can I do a PCB footprint for such a component? Kindly provide a solution to this requirement.
You can't have a footprint with copper on an internal layer, only top and bottom layers. However, you can create a No BOM component that has the copper elements for one internal layer. To do this, create the footprint on the top layer like usual, and then when you import into the PCB layout you can place the part in an internal layer inside the Properties panel. MAke sure to mark the part Standar (No BOM) in the part properties in the library or in the schematic. If you do this then the part can be placed in an internal layer, but the part will not appear in the BOM. When the surface/bottom layer portions and the inner layer portions are aligned, I think you can group them together so that they would all have to move together if you need to change the position.
Another way to do it is to use a design reuse snippet for that part of the PCB layout. If you create a snippet, then you can place it in the schematic and in the PCB layout without having to manually place the parts again, the placement will be copied from the design snippet. There should be documentation on how to do this.
Keepout mechanical layers in the footprint would only be useful as a guide to the designer. You can of course place keepout objects on the copper layers, or all-layer keepouts on the "Keepout" layer, but mechanical layers cannot act as keepouts to copper layers, neither are they able to be targeted by clearance rules (sadly). In the example shown, the keepouts should exist on the top copper layer only, as they are intended to avoid the spring fingers making contact with any surface copper, but should not affect internal/bottom layers.
It drives me bonkers that Altium doesn't include the 3d body projection in the PCB footprint editor. There is no reason why that feature shouldn't exist there so that we can easily add that detail to the assembly layer. I'm not a huge fan of draftsman so I'm creating the 3d body projection in Freecad, exporting it as dxf and importing when creating footprints. Not too cumbersome but annoying enough.
That's a fair criticism for sure, I would like to see something like that in the assembly layer so that you can more accurately draw out the courtyard layer or some other mechanical layer. Luckily some of the footprints you find in the Manufacturer Part Search panel will include this though.
SolidWorks? I looked up the cost of a license for that waaay back when Jamie used it for "Seesaw Saga" and are you $#!tting me?! That's what Adam would call "TV money"! Lots of other software available for creating 3D models for components, and a lot of it is Libre and Open Source. Any basic bitch CAD software will do.
😆😆😆
I'm not a solidworks user or MCAD person, I often just do the extruded 3D body models
Is this an actual person or CGI ?!
I can assure you I am a real person.
@@Zachariah-Peterson Haha, yeah, when i wrote that, the video at it's beginning was in low quality and it felt like a CGI.
Great video though, ty!!