Altium 18 auto compiling in schematic (SOLVED) - Page 1
Forum section: electronics / general

author: mzbas
author_rank: Contributor
timestamp: February 20, 2019, 06:12:06 am
content: Hello everyone, new to the forum and I am in need of your help. I have a big schematic in Altium 18 with aroung 850 components and its sheet size is A. Whenever I do anything, for example move a component the schematic lags for around 3 seconds and I see the message"Compiling xxxxx.Schdoc" in the bottom. I understand that the project auto compiles and runs ERC check in the schematic after any action. This hasn't been an issue with smaller schematics but right now I am unable to work because its stalls everytime i try to do something. Does anyone know how to disable the auto compiling feature. İ know that the online drc for PCB can be turned off in the preferences but I couldn't see how to disable the compiler or ERC for schematic. Thanks in advance for your valuable replies.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 20, 2019, 09:44:03 am
content: Don't think so, but it sounds like a design sorely in need of a hierarchical approach, probably with a hearty REPEAT block.Tim

author: mzbas
author_rank: Contributor
timestamp: February 20, 2019, 10:22:33 am
content: Yes you're right, I may need to change the design but I do like to see everything in a single schematic because I think it makes it easier to debug. Thank you for your advice. If there is a way to switch off the auto Compile/ERC it would still be appreciated though.

author: ddavidebor
author_rank: Super Contributor
timestamp: March 09, 2019, 06:27:46 pm
content: Try opening the schematics alone with no project (only the SchDoc file, close the PrjPcb)

author: mzbas
author_rank: Contributor
timestamp: March 14, 2019, 05:39:12 am
content: Quote from: ddavidebor on March 09, 2019, 06:27:46 pmHi, thanks for the advice. I have tried it, I think it works a little faster this way but didn't quite solve it because its still very slow. Altium still compiles the schematic even when working without the project.

author: Psi
author_rank: Super Contributor
timestamp: March 14, 2019, 06:19:39 am
content: I had this exact problem and fixed it, but for the life of me i cannot remember what the cause/solution was.My Altium project was not super big. Altium would just always recompile for 5 seconds after i changed anything minor, unlike all my other projects which didn't do this.Again, Sorry that i can't remember how i solved it.But one thing i recommend trying is1 ) save/backup your project and files.2 ) Open a new blank sch file3 ) Select all on your current SCH file and copy into the new file.4 ) Repeat the same with the PCB. (select all copy to new file)6 ) Removed the old files from the workspace by closing that project.7 ) Close Altium and Reopen it8 ) See if the problem still exists when opening the new files.Since the new files had default settings and no design rules this will tel you if the issue is some non-default setting somewhere.Then you just have to figure out what rule/setting is causing the problem.(It may actually have been a corrupt file.)

author: mzbas
author_rank: Contributor
timestamp: March 14, 2019, 01:03:08 pm
content: Quote from: Psi on March 14, 2019, 06:19:39 amThank you so much for this comprehensive answer. I have tried it but there doesn't seem to be a difference. I am curious about the solution which you can't remember thought. If you could recall it I would be interested to hear it. Thank you for your help.

author: Psi
author_rank: Super Contributor
timestamp: March 15, 2019, 05:23:47 am
content: So after you moved the PCB and SCH to new files those files still did the recompile thing?Is this happening for you if you change an item on the SCH, PCB or both?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 15, 2019, 08:42:10 am
content: Hmm, adding and removing bits and pieces should be able to binary-search to the culprit.Don't omit things from the search: not just SCH Parts, but SCH sheets in the project, libraries in the project, installed libraries, etc.Tim

author: mzbas
author_rank: Contributor
timestamp: March 18, 2019, 07:00:16 am
content: Quote from: Psi on March 15, 2019, 05:23:47 amYes, it is still laggy after I moved the tranferred the designs to new files. I am only having this lagging issue in the SCH files, because I can shut off the online DRC in the preferences. After I am done with the PCB or need a design rule check I use a batch DRC to see the errors. But unfortunately the schematic compiler doesn't have a shut off option. I believe if it had I could just shut it off and use something like the batch DRC in the PCB and see where the errors are.Quote from: T3sl4co1l on March 15, 2019, 08:42:10 amAccording to what you said I removed my libraries from Altium, restarted Altium just in case, opened up a schematic in the "free documents" and placed around 900 transistors from the miscellaneous library which comes with the program. This component count is about the same as in my SCH file. I thought this approach would isolate the search from any buggy components. In the end when I tried to move a transistor it was still laggy. Which led me to think this lag was perhaps solely from the specs of the computer. What do you think? Is the only way to solve this a hierarchical design with multiple SCH sheets? Thank you for all your responses.

author: mzbas
author_rank: Contributor
timestamp: March 18, 2019, 07:13:37 am
content: As a last attempt before giving up I started messing around with the SCH preferences, thinking maybe the search method you proposed could be replicated for the settings as well. First switching them all off at once, and then one by one revealed the culprit: "Optimize Wires & Buses". Switching off this setting in the General tab under Schematic, seems to remove the lag in the SCH file. Thank you for all your help and supportIf anyone has any further responses or workarounds I would be happy to hear them. Have a nice day

author: mcgilvra
author_rank: Newbie
timestamp: September 09, 2019, 09:29:32 pm
content: Fixed: Had same problem, turning off "Optimize Wires & Buses" did not help. What fixed it was moving BOMDOC into same window as schdoc's or closing BOMDoc.For some reason when I have the project's BOMDoc in a different window from the schdoc's it wants to auto-compile on every sch change. I have a 15 sheet schematic so this was time consuming and annoying to say the least.Reported issue to Altium.