Editor mode in AD17

[Cleaver Greene]

Hi all,
I appreciate that all CAD sw has bugs, or really annoying features, so if something winds you up enough to say I'm going to another tool, no doubt you will find other tools have different annoying features.
That said, I am using altium AD17 and it is getting to the point of making me consider retirement.
I have picked up a design from a colleague who has since left the company.
What he has done is this: He has an "Editor" schematic and two "actual" Schematics that are only visible when you go into cross probe mode.
I'm sure many of you already know this, but my issue is this. The editor mode schematic has an inductor called L10, but the schematics have the same inductor called L12 and L13. For the life of me I cannot fathom the thinking behind this.
I get that as it is an identical circuit, channel 1 and channel 2, you dont want to draw the circuit again, but why not just copy and paste a new sheet in the design, then when I run the BOM, I dont get different components that I see on the Editor sheets.
Then If I do a check for duplicate part numbers it does not find them.
All in All, altium sucks, but probably suck a bit less than others.
How do I get it to check for duplicates?
Regards
Jeff

[free_electron]

that is not a bug. you don't know how the tool works. that's all.

this is a channel based design where one sheet is instantiated multiple times.
Copy and paste means that, if you do a change you need to edit EVERY copy... using a channel based design there is only one document to edit. It propagates automatically.
When exporting the Bom you need to export from the toplevel and select 'Project' as the origin. ( you can export from other origin points but then you get only the parts belonging to that origin. )

[T3sl4co1l]

It's not the clearest feature to the novice, not the most "discoverable" sort of thing.  Though I'm not sure how it could be presented better.  Things to be aware of:
- Re/Compile project after opening (also happens during PCB update)
- See the shadow numbers on designators
- See the extra tabs at the bottom of SCH view

I don't think there's a shortcut or menu option for this Compile View; it's entirely something you have to figure out by eye and mouse.  One of the few things you can't do in multiple ways in AD.

Tools/Annotate gives control over how these (compiled, physical) numbers are assigned, and they can also be customized from Compile View (which will add an .annotate file to the project).  It can be illustrative to generate names on different offsets (e.g. prepend channel index to designator index, R101, R102, etc. --> R1101, R1102, ...; R2101, R2102, ...), though this takes up more space for the labels (if they're placed) and may not be worthwhile in a small design.

Note that, since channels are done by whole components, you can't split parts of a logic gate, for example, across channels.  This maybe isn't surprising, but some other tools do allow this (to varying degrees of success; I recall Multisim always shifting around the designators, making it difficult to keep sync with the PCB!).  If you have extra gate sections you could use, you either need to take those connections up to the parent sheet and put the gates there (or on sibling sheets), or use smaller devices (like the 74HC2G00 and friends), or settle for the waste.

Other not-very-evident things:
- Check BomDoc (if in project) for extended part information, also just generally collecting BOM info better than the Export / OutJob dialog does
- Check Variants for alternate parts/assemblies and DNPs
- PCB: regularly check Project / Component Links; even if everything shows matching, the link codes can get messed up, just popping in and hitting Update can reduce possible spookiness (components not highlighting/cross probing/updating, designators not annotating, etc.).
- SCH<-->PCB updates aren't automatic, you have to use the command.  You don't have to run it; you can use this to view differences in either direction.  Also, updating to PCB is the only one that really works; there's no automatic SCH editing, at best just changing labels/text fields.
- Repour polygons from time to time.  Can be done automatically (Tools/Preferences, Repour Polygons After Modification) but can sometimes accumulate errors that a fresh repour will solve (e.g. overlapped polygons that've poured around each other multiple times).
(Polygons have been historically one of the worst programmed things in the tool; back in the AD10 or so days it could take minutes to repour a complex board.  Just, unconscionably bad scaling.  It was optimized a bit since then, and I forget if AD17 or 18 or which improved it further, but it's reasonably practical nowadays to leave auto-repour on.)

I don't know how much of this is relevant; if you're mainly just viewing and inspecting designs, not editing, don't worry about several of these.  The others, may give you some ideas of where to look to find fab/assy information quickly.

Cheers,
Tim

[Cleaver Greene]

Hi All,
Thanks for the replies.
Maybe I dont know the tool that well then.
I have used other tools where this kind of thing is a lot simpler to do and to understand. AD is just too fancy for its own good.
What I really dont like is the fact it crashes at least twice a day.
Also really simple thing, how come I cant find any way to adjust the font and size of the number of pages and page number?
We use a certain Font for a start, Altium has a default font and size that is not consistant with the rest of the test I am using.
I have gone through every menu I can find and it seems there is no way to change it, not on the template, project paramerters anywhere.
It is such a simple thing to do that AD makes really difficult.
Regards
Jeff.

[T3sl4co1l]

On SCH?  Page numbers and other strings are set by indirection: =SheetNumber for example.

Note that templates can use templates, so you could potentially have to dig quite far to access the actual primitives (text labels).  I think the only intrinsics are the sheet outline, and title block, if enabled.  (Normally you'd draw a company custom template and title block, and use that all the time.)

When texts are accessible (i.e. not in the template), they can be queried with SCH Filter, and edited with Inspector/Properties, or SCH List.  Selection can even be across multiple sheets, so everything can be changed at once, but do this with caution of course.

Tim

[free_electron]

the default is to use the entities defined in the sheet. these are hard coded. Document properties : turn off title block. then design your own. that can be fully customised. remnant from the orcad days...

[Cleaver Greene]

Please could anyone explain why altium does this in Editor  (cross probe mode)?
I have two tabs under my schematic called RMS. RMS1 and RMS2. So these are the same "design" but two exactly the same channels.
As an example I have R139 in the "Editor" tab.
When I look at the RMS1 tab, this Resistor ( and every other component in that sheet) has an extension like this: _RMS1 so that resistor is now numbered R139_RMS1.
When I open the RMS2 tab, I now have R139_RMS2. (And every other component has the _RMS2 extension.
I cannot find any clue anywhere why this is happening and how to fix it.
I tried pasting a picure of this but it doesnt play ball.

Any help gratefully recieved.
Jeff.

[free_electron]

under project options, -> multi-channel tab , change the designator formatting string

[Cleaver Greene]

Hello all,
Thanks for all your replies.
I have found what the problem was, or what was causing it.
The Annotation file. Whether this was corrupt or just plain wrong I dont know.
So I deleted  it and my problem has gone away. No more underscore _part numbers.
KR
Jeff