Newbie to Altium with a few Questions - Page 1
Forum section: electronics / general

author: MatCat
author_rank: Frequent Contributor
timestamp: August 01, 2013, 08:34:51 pm
content: I just pretty much started using Altium, I really like it so far compared to Eagle, though it certainly has some things to get used to!One of my first questions is in 3D mode t renders all of these wierd circles and mil measurements on the copper, how can this be turned off/on?Is it possible to output a high quality render of the 3D board to an image?Also I have a library component I made for the LM2596 which has a fill and vias for the tab of the 263 package to connect to, however there is no way I can find in the PCB Library editor to tell it the via's and fill are GND net (If I go to properties to the Net setting there is no listings to choose), which results in all those via's refusing to connect to my poly fill ground plane on the bottom layer.Thanks in advance for the help!

author: free_electron
author_rank: Super Contributor
timestamp: August 01, 2013, 09:39:09 pm
content: the circles are design rule violations. . fix emalt printscreen for a highres capture, or send it to PDF file in the output jobYou don't assign nets in the library.You don't place vias in the pcb library either.Change the via's to pads. give them all the same number . Remove the fill and place an smd pad with the same pad number as your other pads.so if you have a sot263 with 3 pins. you will have pin being a small smd pad , pin 2 being a large smd pad , pin 3 being a small smd padin the large smd pad for pin2 you place multiple thru hole pads and you also name those '2'.altium will then pick up that this is all the same structure and automatically connect

author: marshallh
author_rank: Unknown
timestamp: August 01, 2013, 11:37:12 pm
content: Design > Reset error markersBut you will still need to run DRC before making gerbers of course, and fix all of them.

author: EEVblog
author_rank: Unknown
timestamp: August 01, 2013, 11:46:27 pm
content: You can turn Online DRC off, and you won't get hassled with those violations. But they are there for a reason. Proper way to do a board is to set your design rules and them stick to them. Any DRC errors showing up should be fix or design rule optimised.For 3D I just use my highest resolution screen and then screen capture. Not sure about the latest versions.

author: MatCat
author_rank: Frequent Contributor
timestamp: August 01, 2013, 11:48:05 pm
content: Quote from: free_electron on August 01, 2013, 09:39:09 pmAhh I see, changing my components to use pads fixed pretty much all of it including the DRC errors (It mostly had no idea what net anything was on and thought it was all cross connecting hehe).

author: free_electron
author_rank: Super Contributor
timestamp: August 02, 2013, 02:30:09 am
content: you can use fills but , after loading the netlist, you need to force an update for the tracks and fills in the partsin pcb :keyboard shortcut : D-N-U Design - Netlist - Update free objects from pads

author: MatCat
author_rank: Frequent Contributor
timestamp: August 02, 2013, 02:46:36 am
content: Ok cool, I actually have the Altium Cheat sheet printed out but damn this software doesn't follow ANY software standards, it's like learning an entire new way of computing using it, but compared to eagle there is no comparison hehe. There is a good possibility I will ask a few more questions on this thread in the near future, though I think at this point I have really gotten down the majority of it (Probably spent about a good week of time figuring it out in total).

author: free_electron
author_rank: Super Contributor
timestamp: August 02, 2013, 03:00:19 am
content: two things to remeber about altium :1 ) if it takes more than 2 mouse clicks or more than 3 keyboard shortcut : you are doing it wrong ...2) this software has a lot of history behind it and a shitload of functionality. most if it not found in other tools.. so yes, it is overwhelming. But hey, if it's good enough to design the mars rovers, the Tesla cars , BMW , SpaceX rockets ... it should be good enough for anyone.

author: Rufus
author_rank: Super Contributor
timestamp: August 02, 2013, 03:31:55 am
content: Quote from: MatCat on August 02, 2013, 02:46:36 amI wouldn't say that. It is quite hot-key driven, partly historical and partly because it is the most efficient way to drive a CAD program.The one really non-standard thing it does is mouse handling. It differentiates between mouse clicks and mouse pressed based on how long you press the button. For example you click an object it gets selected, you hold the button down a bit longer and the object gets dragged it also makes a difference during interactive routing. The annoying thing is that I have never seen that documented anywhere - or that the time difference between clicks and presses is controlled by the windows mouse double-click speed setting. If you set the windows mouse double click speed really fast (because for example you have a mouse with an extra button to which double click is assigned) parts of Altium become unusable.

author: marshallh
author_rank: Unknown
timestamp: August 02, 2013, 03:46:04 am
content: Another thing that I don't remember reading about: the corner or middle of the object you start dragging determins the relative origin.Ex. Drag a resistor on its center origin - it will snap based on that point.Drag from its bottom right corner and that corner will be grid aligned.

author: ludzinc
author_rank: Unknown
timestamp: August 02, 2013, 05:24:12 am
content: Altium has a good tutorial for beginners.Spend the time to run through it and you'll learn 90% of Altium's abilities in 4 hours.It's the first task I give to all my new Engineers.

author: free_electron
author_rank: Super Contributor
timestamp: August 02, 2013, 07:01:28 am
content: Quote from: marshallh on August 02, 2013, 03:46:04 amThat depends on multiple things- where the origin of the part is defined in the library- how the snap filters are set...if you have snap to grid only it will only let you move the part origin to the grid.If other filters are on (hotspot, near aligned, far aligned ) it will let you go off grid. This is intentional. The underlaying reason is the metric components if you are on imperial grid and want to connect or move a metric part you need to be able to go off grid. To prevent having to toggle grids all the time they have these snap filters. Bottom right of the screen. Snap. Click that open. There is a whole list. See what is enabled.

author: MatCat
author_rank: Frequent Contributor
timestamp: August 05, 2013, 06:44:30 pm
content: Lot of great fantastic info here, thanks!

author: MatCat
author_rank: Frequent Contributor
timestamp: August 09, 2013, 07:13:26 pm
content: Ok another question, I submitted my gerbers to ITEAD but they said there was no board outline... how would I do this?

author: David_AVD
author_rank: Super Contributor
timestamp: August 09, 2013, 11:00:48 pm
content: I use the keep-out layer to define a 10 mil outline. Did you draw an outline at all?

author: MatCat
author_rank: Frequent Contributor
timestamp: August 09, 2013, 11:04:35 pm
content: I never drew one, I just used the board size tool.

author: David_AVD
author_rank: Super Contributor
timestamp: August 09, 2013, 11:06:49 pm
content: There you go. You need to define the outline so the board house knows the bounds.

author: MatCat
author_rank: Frequent Contributor
timestamp: August 09, 2013, 11:11:28 pm
content: I see, I assumed that the board size tool did that already! Thanks.

author: tszaboo
author_rank: Super Contributor
timestamp: September 09, 2013, 09:42:07 pm
content: Use some mechanical layer for it. I think default is mech 1. Then add it to all gerbers when exporting. There is an option to do this. Then the outline is clearly on all layer, no confusion.

author: free_electron
author_rank: Super Contributor
timestamp: September 12, 2013, 02:13:34 pm
content: You draw the board contour on the keepout layer.From there you can define rules for pullback per layer.Inner cutouts are also made there. Altium is s amrt enough to figure out the box-in-box so you can have subboards.

author: MatCat
author_rank: Frequent Contributor
timestamp: October 01, 2013, 05:13:29 am
content: Got a new question, PCB thickness, how the heck can I set it for when I do step exports? I am working on a few boards that are going to have cases designed but the problem I am facing is that the step export is exporting a PCB thickness of I think 0.4mm when I need 1.6mm, thanks!

author: tszaboo
author_rank: Super Contributor
timestamp: October 01, 2013, 06:39:28 am
content: Layer stackup manager (shortcut O,K)

author: MatCat
author_rank: Frequent Contributor
timestamp: October 01, 2013, 05:22:46 pm
content: Awesome, worked perfectly thanks!