Altium Tutorial - Page 1
Forum section: electronics / beginners

author: blueskull
author_rank: Unknown
timestamp: September 25, 2016, 11:14:56 am
content: I've made an Altium Designer Tutorial, based on a real word design, a 10kV isolated MOSFET gate driver.Here is part 1, library creation and schematic drawing. The next video will be PCB layout and Gerber generation.https://youtu.be/L_AQ-8GnFrYStill being transcoded, whenever it is ready to watch depends on YouTube.

author: aandrew
author_rank: Frequent Contributor
timestamp: September 25, 2016, 05:45:23 pm
content: Good video, thank you for taking the time to record and upload it!Couple notes though... in layout, you select the parts, the ^C to copy. You get a crosshair which is asking you for the "reference point" for the copy, and you can easily snap to the exact center of a pad or end of a line or, as you did, any arbitrary point. Then when you use ^V the paste center will be that point you selected when copying. This makes it VERY easy to offset pins or perform precise positioning relative to some point. You can also save a LOT of hassle by using the "paste array" when designing the footprints for ICs. The Wizard is the absolute fastest, but using the origin marker with copy/paste and using paste array go a long way in making footprint creation easier.You may also want to make sure the silkscreen widths are compatible with your board house; I tend to make all my silkscreen line widths 4-5mil which works great with most PCB houses, including Hackvana, my favourite board house. I'm a little concerned about how you specify your soldermask expansion to zero; I tend to leave it at defaults which tend to give good results. I don't like soldermask defined pads, which is essentially what you've done by setting the expansion to zero. Some very fine pitch components want this (and others do not) but for the types of components in your video I don't see any clear advantage to this. Having the silkscreen butting right up to the bare copper can also cause problems with placement and reflow.I also am not a fan of the schematic pin order being the package pin order. The schematic is the logical representation of the circuit; if it makes sense to have the logical and physical pins in the same location that's great, but I tend to organize my part's schematic object so that the pins yield to easy schematic "flow". i.e. my power and ground pins are grouped together and (when possible) offset by the amount of space that a capacitor symbol takes, that my enables or other inputs are on one side of the component and outputs on the other, etc.You tend to also shift pads around manually; I like to double-click on the pin and explicitly set the x/y location based on the datasheet. This can get very frustrating, particularly if the datasheet mechanical dimensioning requires you to go through a lot of mathematical gymnastics to arrive at the correct dimension. It does pay off though by ensuring the footprint will match the part. This is helped a lot if the center of your footprint is at (0,0) too, because all the pin dimensions tend to be centered on the origin. You also seem to deviate from the recommended PCB footprint for unexplained reasons. My experience has shown that their recommended footprint often gives you the best mechanical connection and you should only deviate from it if there is a very good reason to do so. This is particularly important for fine-featured parts where they have specific soldermask or pad dimensions to ensure high reliability during assembly.I've recently fallen in love with the 3D footprint feature. A LOT of vendors are providing IGES or STEP files of their components. This is particularly awesome when the datasheet has incomplete or missing footprint recommendations. You can use the 3D file to instantly tell if the part and footprint are compatible.One final note/suggestion... if you move the footprints and schematic symbols so that the center is aligned with the center of the grid you will find that rotating and flipping the component works much better, in that it won't "jump" in annoying ways.I'm looking forward to the layout tutorial. :-)

author: aandrew
author_rank: Frequent Contributor
timestamp: September 26, 2016, 01:39:12 am
content: Quote from: blueskull on September 25, 2016, 10:31:27 pmI used to do that but ran into tombstone issues; I will do VIP down to a ground plane before I will use a solid polygon connection on one side of a passive; both sides is fine in my experience.QuoteThat's the great thing about this, there are a lot of different ways to getting things done.QuoteInteresting; I've never had this issue, but in the schematic editor my symbols all have pin/body lengths that ensure the pins terminate on-grid. In layout I've never had an issue, but like you mentioned above, there are different ways to getting things done and whatever works, works. :-)Thanks again for the video, will keep my eye out for the layout video.

author: Wilksey
author_rank: Super Contributor
timestamp: September 26, 2016, 10:22:21 am
content: Not a bad tutorial,I think one piece of information missing that might have been useful is part creation, i.e. multi part gate, or split part micro.A few other things that get asked a fair bit are:1. How to draw an active low pin name (with the bar on the top of the name)2. How to make pins with the same name, i.e. a micro with multiple VDD pins, do you name them all VDD, or like in other packages, VDD1, VDD@1 etc3. How to assign multiple footprints to a part (DIP and SMD for ex)Anyway, thanks for making the tutorial(s)!

author: aandrew
author_rank: Frequent Contributor
timestamp: September 29, 2016, 04:27:50 pm
content: Quote from: Wilksey on September 26, 2016, 10:22:21 amI used to like the overbar notation, but have moved away from it. I find that the overbar is easy to "lose", either through poor eyesight or printing or low resolution, etc. My personal preference now is for the trailing octothorpe (#) and, as a distant second, the trailing slash (/), although I feel that it's less "in your face" as that fat octothorpe.

author: Wilksey
author_rank: Super Contributor
timestamp: September 29, 2016, 05:20:32 pm
content: If I don't use the "proper notation" I get other, angry engineers ranting at me.I know how to achieve all of my questioned items, I was pointing out that it might be worth including them as people moving away from other packages might need to know, I know I did when I first started using AD!So...2. would be useful to add to your video, even if you only spend a few minutes on it.3. You can add multi footprints / technologies (an EAGLE term) to the schematic symbol quite easily, it might be worth, covering a SOIC and DIP example in your video.When I say add to your video I mean a new video covering the features.Another sub video which would be useful (Again, would have saved me days back in the day) is simple "high speed", length matching and differential pair (and multi differential pair) routing, again, doesn't have to be a 30 minute long feature!Good content so far though!

author: rdl
author_rank: Super Contributor
timestamp: September 29, 2016, 05:29:50 pm
content: Quote from: blueskull on September 25, 2016, 10:31:27 pmI am the same.It always seems to me that using "function-centric" parts for schematic results in more of a block diagram, but with "chip-centric" I can be thinking of physical circuit layout from the start.I only make simple things though. I'm sure both methods have their place.