New to Altium - Page 1
Forum section: electronics / general

author: AgileE
author_rank: Contributor
timestamp: October 22, 2018, 01:30:35 am
content: A few observations, I've recently switched from Eagle to AD18 (I did not like the changes to the Eagle purchasing model). After a couple of months using it, while the basics are reasonably straight forward there are quite a few 'odd' issues I'm having with the interface, mostly usability and the seeming lack of features that should be there;1. Holes - a pad, really the only way? Seems kinda silly. I had to look up how to add a simple hole in the PCB. Easy enough once you know - but counter-intuitive.2. PCB layout for fabrication. Pretty much all the boards I make are panalized, often with a combination of tabs, V-grooves and tooling strips. I would guess that is how most boards are. So the question is why are the tools for board layout either missing or so painful to use it is like having a root-canal? This seems to be a failing for most CAD packages. I was hoping Altium would be better, it is better than Eagle at this, but still, either I'm doing it wrong or it is nowhere as efficient as it should be for a process that I'd expect the majority of designs to require.3. Thermal balancing of poly-pour connections. The options are none,two or four connector styles. When using heavy multi-layer boards with plenty of thermal mass it would be nice if there was an option of a single connection. It would be really nice if it was even a little smarter and based the thickness of the connection on the size of the other connections used by the component's other pads. This would mean that I could actually let the pour handle the connections itself, rather than setting it to no connection and manually adding it. This is to help reduce tombstoning of smaller passives on 'thermally' challenged boards.4. If you use the job outputs panel to create the Gerbers etc. then there doesn't seem to be any way to also incorporate any panel routing etc. that would be done via 'CAMtastic', which while it is no great loss it strikes me as though the whole board fabrication effort is a bit of an 'add-on'.5. The Documentation is sadly lacking. I've never actually found the answer to any question I had via the Altium web pages documentation. It's always found via Google from forums etc.6. Replacing a part in the schematic. Even if its the same footprint, is delete+add the only way to do this? What a pain. One new simple menu option to replace would be a god-send. It's even more important if using supplier linked parts where a change in value results in a different component.Any other issues converts have found?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 22, 2018, 02:49:54 am
content: Quote from: AgileE on October 22, 2018, 01:30:35 amA via, I suppose (but those are always plated). Otherwise, Place / Board Cutout. Remember to put an outline on your board outline layer (usually Keep-Out or Mechanical 1, I think in AD18 that's more explicitly not what K-O is for, anymore?) just to make sure the fab knows about it.QuotePersonally, I never panelize, either because it's a proto that it doesn't apply to, or because assembly will handle it however they see fit. (I think most of the time, they do in fact panelize; and they have better tools to do it their way, anyway.) At most, I put some suggestions on how to prefer panelization and cutting (e.g., mostly routed board outline, with tabs + score for easy release). YMMV.A lot of fabs will panelize for you, too, although I don't know if that's a free service on already-expensive fabs, and cheaper fabs will charge more for that (or just do it badly besides).CAMtastic is definitely a 1998 dated pile of crap, though...QuoteI guess I'd be worried if, due to fab error or later mistake, that single spoke gets broken.What's wrong with using thinner and longer spokes?Spoke dimensions are controlled by rule, which is more trouble than Eagle, or say Ultiboard, where you can set it however. But it is more powerful. Much of Altium is that way, and yeah, it's a different system to get used to. The query system in particular is steep, but extremely powerful for setting rules, and navigating large designs (via the Filter panel and such).To control spoke size based on pad size, use a query like:(AsMils(PadXSize_AllLayers) > 60) AND (AsMils(PadYSize_AllLayers) > 60)and set it to, say, 10 mils default, 20 mils (passing this rule), and so on.Note that objects drop out of scope after the first rule match, so you can set a rule for, say, 100 mil pads, with the highest priority; then another rule for, say, 80 or 60 mil pads, and so on down the line. You don't have to define perfectly exclusive sets (i.e., 60 to 80 mil pads only).This is also bothersome for setting net-to-net clearances, but it is what it is. (For that, you'll usually set a Net Class, and set a rule for spacing between nets in the same class, and between that class and nets NOT in that class.)Speaking of which, learn classes too -- most often, net and component classes. You won't always need them, but they're great when you do.QuoteYeah, you can't job-generate outputs from CAM. CAM is really only an inspection tool, to view outputs, not the other way around. Even though it can do more things, but not very well. (Don't you just love programs that do that?)QuoteMeh, hit or miss I'd say, with more things being hits than misses? The problem may be, because you don't know how to do things, or how things work, you're searching on what you want to do -- but documentation isneverwritten that way, it's only ever documenting what the thing does. Definitely not what itdoesn't.Sounds obvious and dumb, but the utter lack of explanation and thought that goes into most any documentation, for most any program, is trulying.So you have to search for a post that someone else may've written, asking how to do something, and if it can be done a certain way, or not at all even, and sometimes you find this even for something so obvious that they had to have done it, yet didn't...You'd expect more from a $5k+ piece of software, but, ah, price doesn't actually mean anything. You will find, as things get more expensive, so does its support. (No one buys a BMW because they want less, and cheaper, repairs. Oh my, no.)On the upside, you've got that one year free subscription. Call them up. (Don't like making phone calls? Tough..)QuoteOpen the component dialog, see the Link to Library Component section. Enter a new ID, or Choose... from the list of installed libraries (you can have project-specific libraries, Installed (global to the installation of AD), and libraries on a Path). Warning: choosing a new component replaces all parameters but the designator and comment!A lot of things aren't worth keeping unique library items for, or it's a matter of preference. Example: generic resistors. For SPICE purposes, set the Value parameter and you're done. For BOM purposes, set the required parameters (maybe Value, and set Comment or Description to some useful data, like type (e.g. "1206 5% 0.25W 1k"), or MFG/PN, or whatever), or apply a Supplier Link (from the Supplier Search panel), or link it to a part number spreadsheet (via database link library or something) from which it pulls all the necessary info, or...Tim

author: mrpackethead
author_rank: Super Contributor
timestamp: October 22, 2018, 02:56:15 am
content: Quote from: AgileE on October 22, 2018, 01:30:35 amdont' attempt to use camtastic. You can embedd a pcb into another file, tell it how many you want in the array etc, adjust the rotations.. Then draw in your v-scores, tabs etc as required. Its one of the things it does quite well.

author: AgileE
author_rank: Contributor
timestamp: October 22, 2018, 03:21:48 am
content: Quote from: mrpackethead on October 22, 2018, 02:56:15 amYep, that's what I do some times... but it's a lot of repeated work for complex panels. What I've ended up doing then is putting part of the routing/tabing in the single board file, with a minimal surrounding PCB (with no Mech 1 boarder), then embedding that with the embedded array tool. It works but it's not ideal as part of the manufacturing layout ends up in the basic board design and it's not so good for designs with tabs between boards without a support strip separating them. It bugs me that such a fundamental part of the design process is not well catered for.

author: mrpackethead
author_rank: Super Contributor
timestamp: October 22, 2018, 04:13:12 am
content: you can embed two things at the same time. create the tab routing in one file and the pcb data in another. Works well

author: radar_macgyver
author_rank: Frequent Contributor
timestamp: October 22, 2018, 04:53:31 am
content: Quote from: AgileE on October 22, 2018, 01:30:35 amView the part properties, there should be a "Design Item ID" property with an ellipses button ('...'). Clicking that should bring up a library browser from which you can pick your replacement part.

author: AgileE
author_rank: Contributor
timestamp: October 22, 2018, 04:53:56 am
content: Quote from: mrpackethead on October 22, 2018, 04:13:12 amThat could work with a bit of thought, I'll give it a go.Ta

author: AgileE
author_rank: Contributor
timestamp: October 22, 2018, 04:56:33 am
content: Quote from: radar_macgyver on October 22, 2018, 04:53:31 amAh, I'd seen references to editing the item ID, but looked like it needed a few extra steps, perhaps that was in an older version. This sounds more like what i'd expect from a 'replace' menu option.Thanks

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 22, 2018, 02:08:01 pm
content: Mind that, if a library is ticked, it will search for the new ID in that library, which if you're pulling from a different one... So, just untick or change that field too. (It only has to be ticked, and set to a specific lib, if you have parts of the same name in different libs in the current project/install.)You can even do this from the SCH Inspector panel to change parts en masse, or maybe even from the spreadsheet view, not sure, I never tried that.Tim