Am I a noob or are they just really smoking crack at Altium HQ?!? - Page 1
Forum section: electronics / general

author: TnF
author_rank: Contributor
timestamp: March 14, 2021, 10:50:24 pm
content: For the love of the impedance matching gods i cannot seem to find a way to achieve the following in the latest release of Altium Designer:-Square track ends: This seems to be locked internally and there is no way other that to overlap the track with a pad of the same width. Technically you should be able to select any type of shape for a track end (semi-circle, square, triangle, polygon, custom shape)-Convert track to pad: Much like other types of possibly useful conversions they are missing.-Flip board (view) horizontally in 2D/3D layout mode: Again you are locked internally into only having a flipped board view on the vertical axis. There is no way to mirror on the horizontal axis. On 3D layout mode you can at least rotate the view 180 degrees to achieve the desired view.-Solder mask expansion for text: This option is non-existent at all. I found no way to expand the solder mask for text on copper even if i tried using the rules. This applies to stroke text as well. The only workaround i can think of is to duplicate the text with thicker stroke width and paste it in the solder layer. This will work only with stroke text, for other types the only way is to import the text from AutoCAD as primitives, or as a graphic.-Explode text to primitives: Again missing.-Arrays: Unless you want to do penalization of a completed pcb you are out of luck. Lets say you want to duplicate a component/primitive and space it at a specific pitch, it's either manual work or import from AutoCAD.-No actual pad import options for AutoCAD: If you wanted to array pads in AutoCAD and for the above and then import them you are again out of luck.-Mirror/Rotate imported graphics: No way to do it inside Altium but can be done externally with an image editing program prior to the importI've probably left a dozen more missing BASIC features behind, so AM I THE NOOB or are they smoking the good stuff over at Altium HQ?

author: penfold
author_rank: Frequent Contributor
timestamp: March 15, 2021, 12:09:02 am
content: Not by any chance from a Proteus background are you? Reminds me of stuff that I was used to doing in proteus years and years ago and Altium wouldn't let me.With "convert track to pad" what's the end goal there? You can create an arbitrary pad in footprint editor using a region, still a bollocksy implementation,For arrays, for primitives/pads/holes and stuff... its possible to do with the scripting interface and I think there's an example for it,PS, the subject line just sums up so much about Altium!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 15, 2021, 04:59:58 am
content: Quote from: TnF on March 14, 2021, 10:50:24 pmPossibly you could hack this in CAM, by changing what aperture is used to draw the shape.I don't know for what purpose this would actually be useful, at worst an aesthetic or technical annoyance?QuoteAs mentioned, the traditional way to draw pads is to place regions around a small logical pad, and they will connect when placed on PCB. Set all the usual pad properties, i.e. soldermask and expansion, paste if applicable. I think you can draw pads directly too now, I just never bother using it. As usual in Altium, there's about three completely different ways to accomplish the same thing.QuoteDon't know what good this is, it seems it would reflect more on your spacial reasoning ability than the system itself? Maybe that, in itself, is an argument in favor of such a feature -- why restrict usage from those with poorer spacial reasoning. Then again, maybe it would just get super confusing? Would need to draw axis vectors on screen (i.e., even in 2D).A hack around this, is to select all and rotate manually. You are actually modifying the design in this case, so make sureeverythingis in fact selected, even locked, transparent, shelved and otherwise differently- or in-accessible (board edge?) objects. Don't expect things to remain perfectly snapped to grid, everything may end up out by 0.001 or something. Can also do arbitrary angles, and can set arbitrary grids, albeit to some degree of bother (don't forget to rotate any local grids you've set up, too!).QuoteStroke text could be exploded to shapes, they're clearly drawn specially in that way; I don't know why they don't have that feature (or they do and I haven't checked). TrueType fonts obviously cannot, not without grossly approximating them as arcs or tracks.The hack I use is to use the OCR A Extended font, and make positive and negative copies. I like to do positive in silkscreen, negative in copper, and nothing in soldermask; at 1oz copper, the silkscreen just fully sinks into the void left in the copper, making a very smooth and indelible mark. Probably some self-alignment on printing, too.I don't know what good, soldermasked text is. Text usually looks terrible as pads, it gets globbed up with solder. I suppose it may look better e.g. with ENIG when masked during wave, or non pasted. In which case the accidental drop shadow created by mask misalignment is annoying.And for the same reason (TrueType) I imagine, expansion cannot be calculated, at least not trivially.You can always draw them in a compatible vector format and import as arcs/tracks. Or bitmap and import as tracks or dots (yuck, though).QuoteHmm, have you tried Paste Array?Or for more complicated structures, multichannel with Rooms?Still a lot of manual work, wiring up the connections to and from the channels, but what do you expect, it's a lot of components en masse, you have to put in some work. Set up the autorouter if you find it such a pain to do manually.QuoteYou could draw and import a fiducial pattern, and rubber-stamp your objects on top of it; but yeah, nothing like that.Oh! Or instead of multichannel, you could go as far as making a whole ass footprint, and repeating the component in the respective locations and rotations. This can be pasted in via PCB List panel. Obviously, using a footprint sacrifices many PCB features (namely things controlled by routing, and design rules besides just checking for errors), and is more annoying to change.Quote??Mirror, drag and press X or Y (there's both axes this time!). Rotate, there's a command (M, O). Use that all the time.QuoteBASIC is available as VBScript support...Mind, they probably are smoking things, do not take this reply as any contradiction to that possibility.Tim