diptrace schematic confusion - Page 1
Forum section: electronics / general

author: Chopsticks
author_rank: Regular Contributor
timestamp: January 27, 2013, 07:28:32 am
content: ive been using eagle for a little while and although im able to make layouts etc pretty well i recently found that i was running into problems due to board size (pin count was fine but i just wanted to spread things over a larger area for enclosures and so forth). anyway after doing my head in trying to work out eagles ridiculous upgrade paths not to mention the cost i decided to give diptrace a go.ive only been fiddling around with diptrace the last day or so and it seems to be pretty good however theres one thing that is annoying me. in eagle's schematic layout when i add a DIP package for say TL072 it actually placed a dip package with all the pins, i prefer it this way. however in Diptrace it places 2 different sections to the IC as well as a separate power and ground section. ie it shows 1 Dip package as three separate 'parts' or what not in the schematic editor. Is there a way to globally change this to just show the IC as 1 part on my layout?i hope im making sense if not i can probably upload some photos when i get back in the lab to further explain

author: Chet T16
author_rank: Frequent Contributor
timestamp: January 27, 2013, 09:16:44 am
content: I wasn't sure what you meant so i checked it out, screenshot attached.

author: Chopsticks
author_rank: Regular Contributor
timestamp: January 27, 2013, 09:49:08 am
content: yes that what it looks like to me too, but in eagle they just use one icon for the whole 072 etc. is there a way to change this in diptrace?on another note, why is diptrace missing so many patterns for parts, for example i cant find a single variable resistor that has a pattern rendering doing a pcb layout useless

author: Mechatrommer
author_rank: Super Contributor
timestamp: January 27, 2013, 11:13:02 am
content: Quoteweird! from the start i followed the tutorial, it has been like that, ie creating one dip package. creating multiple separate opamps in that package is something that i have to learn it myself later. look at the attached images, the first is my older 2 opamps ic in one package, good for drawing schematics that closely resembles physical form albeit "spaghetty" looking. later i figured out everybody are using standard opamp symbol for their schematics, good for true ee understanding, sharing and documenting, so later, "slowly i turn" to update my library to use multiple separate objects in one package (2nd attached image). obviously diptrace can do both.

author: Chopsticks
author_rank: Regular Contributor
timestamp: January 27, 2013, 05:17:35 pm
content: see i wouldnt mind to much if the power/ground rails could be connected but it doesnt seem to let me, i do understand to reasoning to 'split' the op=amp into its logical form but from a schematic point of view (and maybe its just me) but i kind of prefer to keep it as 'one' part just to make reading it easier on the eyes...perhaps theres an option to choose the default viewing mode, might have to give them an email and enquire

author: Mechatrommer
author_rank: Super Contributor
timestamp: January 27, 2013, 07:01:11 pm
content: maybe you use different steps when creating new component? mind to tell us how?

author: codeboy2k
author_rank: Super Contributor
timestamp: January 27, 2013, 08:31:45 pm
content: Quote from: Chopsticks on January 27, 2013, 05:17:35 pmA schematic is far easier to understand when it is drawn logically, not physically, using the component forms like that, not physical forms. Leave the physical layout to the PCB editor.I once saw a guy's schematic drawing, it was about 50 x 7400 series chips.. every chip was laid out like the physical devices, pins numbered sequentially from 1-14 and 1-16, etc. ... drawings of rectangular chips with hex invertors, 8 buffers, 2 flip flops, etc.. all neatly held within the confines of their physical part, and wires criss-crossing all over the schematic back and forth just to hit a part.As mech said, it makes for spaghetti schematics. It was really hard to see a logical flow of data when drawn that way.At PCB layout time you can pin swap to make layout easier. I almost think schematic editors should never have pins on them, just logical functions that can be assigned at layout time, but that's not always going to work out for some parts.

author: Kremmen
author_rank: Super Contributor
timestamp: January 28, 2013, 04:58:22 pm
content: Quote from: Chopsticks on January 27, 2013, 07:28:32 amNo there isn't (a global way). Once you get more experience, you will want to do it the way DipTrace does it. That is the way it is done. In more complex schematics the multipart presentation is almost necessary to keep the circuits understandable. Really, do switch your head into that model, you will be happy you did.2 opamps in one package is easy, but what about a big FPGA in a 400+ ball BGA package? Do you really want to show that as one enormous rectangle with a huge forest of pins radiating in all directions? I think not.

author: Mechatrommer
author_rank: Super Contributor
timestamp: January 28, 2013, 05:43:23 pm
content: Quotedont FPGAs are generic type of chip? similar to mCU? i mean each pin can be anything depending on the program. so i still have this in my mind for such generic (programmable) device, i'll do it in one single box radiating pins (or buses better i think), i think its better than 400+ logic gates scattered around, no?

author: Kremmen
author_rank: Super Contributor
timestamp: January 28, 2013, 06:16:41 pm
content: While there might not be a single right answer for every occasion, some kind of structured approach will beat a mass of undifferentiated pins every time. You could separate the component into e.g. power inputs as one part and each I/O bank into separate parts. Or some other scheme based on what you want to highlight in the schematic. I tend to have multiple symbols for parts like these, and pick the one that seems most appropriate for the case.Another pet frustration of mine is the habit of some people in drawing logic components. Elementary gates are shovelheads and all else is blank boxes with nothing whatsoever to indicate the inner workings of the chip. Its almost like nobody ever heard of IEC and the symbol presentation standard. Or then it is too difficult to bother - easier to just draw a blank box...P.S. I attached a couple of often used symbols of mine, familiar to most of you. The left one is a 74595 serial to parallel latch and the right one is one version of a 74165 parallel to serial one. Both are drawn to IEC recommendations. Once you know how the IEC symbology works, you don't really need the data sheet any more. It is all there in the symbol. Take the 595: You can immediately see that there are two 8-bit registers (1D and 2D), bit-connected in parallel, but each with their own control logic (box with narrowed foot on top of each register).The first one is an8 bit shift register (SRg8). The internal state is stored by the individual elements (D). There is a reset input R (active low as indicated by the arrowhead in the pin, and (rising) edge sensitive shift clock input (first clock - C1) as indicated by the clock symbol > next to the input, and shift symbol -> in the control block.The second one is an 8-bit data register clocked by input C2 similar to C1, and there is an active low Enable signal that controls the 3-state outputs (indicated by the small inverted triangle next to the first output - implicit repetition if not otherwise indicated). The supply lines, while not strictly a part of the symboil, are there to simplify drawing, and suggest the proper connection by their placement. The 165 works similarly, except here i have separated the control block to make it easier to connect the bus part and control part separately. This version has one weakness, the power pins are laid stupidly because they separate and that should be fixed. But you get the point.

author: Kremmen
author_rank: Super Contributor
timestamp: January 28, 2013, 06:53:18 pm
content: Quote from: Chopsticks on January 27, 2013, 05:17:35 pmThe symbol is drawn stupidly. The power connections are already there in the rectangular part, you don't need the useless tails in the amp symbol for anything. This is one point of multi-part symbols; now you can take the supply wiring elsewhere in the schematic, away from confusing the actual amp part of the circuit.

author: Chopsticks
author_rank: Regular Contributor
timestamp: January 29, 2013, 01:50:00 pm
content: thanks for all the input everyone, the more i think about what you guys are saying the more it makes sense, i shall go adjust my habitsthanks again for all your help