Author Topic: Altium Tutorial  (Read 7601 times)

0 Members and 1 Guest are viewing this topic.

Offline blueskull

  • Supporter
  • ****
  • Posts: 12343
  • Country: cn
  • Power Electronics Guy
Altium Tutorial
« on: September 25, 2016, 11:14:56 am »
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-8GnFrY

Still being transcoded, whenever it is ready to watch depends on YouTube.
« Last Edit: September 25, 2016, 10:15:18 pm by blueskull »
 
The following users thanked this post: SeanB, Wilksey, thm_w, fubar.gr, evb149, continuo

Offline aandrew

  • Regular Contributor
  • *
  • Posts: 229
  • Country: ca
Re: Altium Tutorial
« Reply #1 on: September 25, 2016, 05:45:23 pm »
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. :-)
 

Offline blueskull

  • Supporter
  • ****
  • Posts: 12343
  • Country: cn
  • Power Electronics Guy
Re: Altium Tutorial
« Reply #2 on: September 25, 2016, 10:31:27 pm »
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.

Correct, I forgot to mention the copy origin point. I do not use wizard unless making BGA packages because by drawing pads individually, I have a second chance to double check datasheet and start planning placement and layout.

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 use direct poly pour for lowest possible inductance and resistance, hence NSMD always result in larger ground than other pads. Therefore, I use SMD all the time except for super fine pitch QFN and BGA.
When doing fine pitch designs, I will use NSMD pads, and set tules not to poly pour these parts, then I will finish GND connection myself.
OSHPark can produce SMD design easily down to 0.5mm pitch QFN and 0.8mm pitch BGA according to my experience.

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.

Many people don't like my schematics style, and I can understand it. My idea is my SCH layout is almost PCB layout in terms of parts affinity and pin assignment, so that I can start planning PCB at the earliest possible stage.
I spend much more time on planning than actually CAD drawing, and I always plan while actually drawing.
Only when working with large packages such as packages having more than 100 pins I will use logical symbols, simply because drawing everything together will screw up aesthetic a lot.

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 have my pinky finger on CTRL almost all the time and I use CTRL+M and CTRL_ARROWKEYS a lot. I guess it is just I'm used to do this, but both methods should work.
My keyboard has CTRL key in CAPS LOCK position, so resting my pinky finger on CTRL is easy.

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.

Correct. I don't so this is because I'm lazy, but if I am to do a commercial presentation, I will do my best to get the most beautiful 3D render.

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.

Yes, but I want consistency in SCH and PCB. In PCB, sometimes Altium will cause pad off-grid error that cannot be aligned if the origin point is the center of the part while the length/height of the part is not 2N times grid size.

I'm looking forward to the layout tutorial. :-)

Will film it soon, should upload it by tonight. I have a mid-term tomorrow, so I will try not to sleep too late.
 

Offline aandrew

  • Regular Contributor
  • *
  • Posts: 229
  • Country: ca
Re: Altium Tutorial
« Reply #3 on: September 26, 2016, 01:39:12 am »
I use direct poly pour for lowest possible inductance and resistance, hence NSMD always result in larger ground than other pads. Therefore, I use SMD all the time except for super fine pitch QFN and BGA.
When doing fine pitch designs, I will use NSMD pads, and set tules not to poly pour these parts, then I will finish GND connection myself.
OSHPark can produce SMD design easily down to 0.5mm pitch QFN and 0.8mm pitch BGA according to my experience.

I 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.

Quote
Many people don't like my schematics style, and I can understand it. My idea is my SCH layout is almost PCB layout in terms of parts affinity and pin assignment, so that I can start planning PCB at the earliest possible stage.
I spend much more time on planning than actually CAD drawing, and I always plan while actually drawing.
Only when working with large packages such as packages having more than 100 pins I will use logical symbols, simply because drawing everything together will screw up aesthetic a lot.

That's the great thing about this, there are a lot of different ways to getting things done.

Quote
Yes, but I want consistency in SCH and PCB. In PCB, sometimes Altium will cause pad off-grid error that cannot be aligned if the origin point is the center of the part while the length/height of the part is not 2N times grid size.

Interesting; 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.
 

Offline blueskull

  • Supporter
  • ****
  • Posts: 12343
  • Country: cn
  • Power Electronics Guy
Re: Altium Tutorial
« Reply #4 on: September 26, 2016, 09:17:43 am »
And here comes the second and last video of this series. I will probably post video 0 (intro and design) tomorrow, but I'm not sure as it has some sensitive information, and I have to cut them out, that takes time to do.

https://youtu.be/hTth3ocYMEs

Still being transcoded, whenever it is ready to watch depends on YouTube.
« Last Edit: September 29, 2016, 05:31:26 am by blueskull »
 
The following users thanked this post: thm_w

Offline Wilksey

  • Super Contributor
  • ***
  • Posts: 1153
Re: Altium Tutorial
« Reply #5 on: September 26, 2016, 10:22:21 am »
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 etc
3. How to assign multiple footprints to a part (DIP and SMD for ex)

Anyway, thanks for making the tutorial(s)!

 
The following users thanked this post: blueskull

Offline blueskull

  • Supporter
  • ****
  • Posts: 12343
  • Country: cn
  • Power Electronics Guy
Re: Altium Tutorial
« Reply #6 on: September 29, 2016, 05:34:45 am »
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 etc
3. How to assign multiple footprints to a part (DIP and SMD for ex)

0. Split part: will add to my future video.
1. Negation: will add to my future video.
2. Same label, different designater. I do not know if Altium can automate this. I do this manually all the time.
3. I always create a SCH library with one footprint, then when needed, assign another package manually in SCH editor.
 

Offline aandrew

  • Regular Contributor
  • *
  • Posts: 229
  • Country: ca
Re: Altium Tutorial
« Reply #7 on: September 29, 2016, 04:27:50 pm »
1. How to draw an active low pin name (with the bar on the top of the name)

I 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.
 

Offline Wilksey

  • Super Contributor
  • ***
  • Posts: 1153
Re: Altium Tutorial
« Reply #8 on: September 29, 2016, 05:20:32 pm »
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!  :-+
 

Online rdl

  • Super Contributor
  • ***
  • Posts: 2671
  • Country: us
Re: Altium Tutorial
« Reply #9 on: September 29, 2016, 05:29:50 pm »
Many people don't like my schematics style, and I can understand it. My idea is my SCH layout is almost PCB layout in terms of parts affinity and pin assignment, so that I can start planning PCB at the earliest possible stage.


I 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.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf