slow system from sw2018 to sw2019

[vinci16]

good morning to all, yesterday I installed the 2019 version of solidworks on my pc, I press that with the 2018 version, despite I do not have a high-performance processor, I have never encountered great problems (by understanding: I have an intel(r) core(tm) i7-7500u from 2.70 ghz dual-core 64-bit). Today I try to open one of the usual assemblies with the 2019 version and I find myself a huge slowness of the system that occasionally gets stuck due to the use of 100% of the cpu.
I would like to understand, is it normal a difference so marked by a version to the previous one?
Thank you for your help.
a greeting

Andrea

 

[meccanicamg]

normal for two reasons: heavy version because new, heavy load because it still has to convert the previous version files.
try to make a copy of everything, save everything and reopen, you would see that it takes less the second opening after saving in current version.

 

[vinci16]

thanks, I confirm that the speed has increased a lot once saved the file as a new and reopened version.

 

[vinci16]

Good evening to all, I thought I solved the problem of slowness but it wasn't like that.
I'll explain better.
- use for the 2019 solidworks university sp2.0 student edition (the previous version was solidworks 2018 sp 3.0 and, absurdly, worked faster)
- I open 'assieme' files that contain parts of 'previous versions', saving the 'assieme' file I was convinced that all 'part' files in the various subassiemi were also converted but I realized that some parts are still of previous version. (Is there a way to save all sub-parts and sub-assiem without having to open them once? )
- I went to a more performance pc to try to solve the problem of slowness (a workstation lenovo thinkpad p53 that mounts intel i9 9880h processor and rtx picture 4000 video card) but I still feel slower than the system. in particular, passing from a set to a subaxieme or providing different basic commands, the 'cler' appears on the sw icon and the message that "solidworks is occupied with some type of command provided".

I wonder if the system is set correctly but I can't find answers that can change the situation.
Thank you in advance for the help provided.

Andrea

 

[MassiVonWeizen]

there are various settings to improve performance. I've written a lot on the forum. do a search
the base however is modeling well controlling the times of reconstruction (a trivial error little considered is to make repetitions of the functions with the geometric repetition mode inserted even when not needed).
if, for example, to make a sheet, as in another your request, you pass through the transformation of solid multiply the functions and consequently the time of reconstruction of the particular.
a sketch too elaborate with included bevels and rays takes more time than a simple sketch and a function for bevels and one for rays.
start checking statistics, you may have surpriseshttp://help.solidworks.com/2019/italian/solidworks/sldworks/hidd_feature_report.htm

 

[vinci16]

Hello, thank you for your answer. definitely have certain parts created as you say 'not in the most correct way' possible slows down the system. I will certainly try to improve it! evaluating the performance I noticed that some files included within the axieme have a certain length of opening due to geometric complexity or research within the toolbox of sw. some of these I will be able to "lighten" as we said before, while others are provided to me by my professors, why they will have to stay.
right today I noticed that after doing all the update of windows and graphics card the situation has improved considerably.
to open a set of 3500 parts about 40 seconds (I assume it is a good working time).
I now ask a further question, as I complained earlier that: opening a set comprising sub-axis and therefore parts belonging to a previous version and saving this macro-axis, not all the parts contained are overwritten in the current version. Do I have to activate some flags that allow me to extend the rescue in the current version to all parts included?
Thank you for your help.
a greeting

Andrea

 

[MassiVonWeizen]

generally solid saves or requires you to save all files that in your opinion have been updated; how to impose on him to save all the files regardless sincerely I do not know if it is possible.
if all the files of the axieme are in the same folder you can use the task manager or planning utility to save all the files in sequence, maybe while doing anything else or you are on break.
if the files are in separate folders I don’t know if it is possible without using a macro (this save out all part components with specified extension could, for example, do the case)

toolbox components are a tool of the devil. would be burned in public at the cry of I'll handle it.are of a hallucinating heaviness, full of equations, made with the same logic of a bonobo under lsd, capricious as a schoolgirl in full hormonal storm.
if you have to use them the first thing to do after you have created them and save them by name and then disconnect them from the toolbox world with the utility Setdocprop.exe; Finally open the part and eliminate all the equations and functions suspended.

 

[vinci16]

Unfortunately, the files of my group are all grouped into a folder that owns subfolders, containers of the files part or together.

I fully agree with your reflection on the elements of the toolbox, this is obscene stuff. every time I understand that I have to use elements included in the toolbox I realize them from me, such as screws, nuts, bolts. Turns out I've missed a seeger on the street :roflmao.
I will make it as a part and therefore avoid having to move from the toolbox.
Thank you for your answer.
a greeting

Andrea

 

[MassiVonWeizen]

screws, dice, rosettes you can do them quietly configured with the data table.
for these types of files if for any kind you start from a common base you can create a file by type so you can replace it in the assemblies without problems losing mating.
example:
Type: screw
typology: hexagonal head, cylindrical head, vased head
create a file that you will use to make 3 types, then model your common base, here I will mark you 2 types of modeling that you can use
1. (that technically correct) create a plan and an axis that you will then use to make matings; by this method any solid you go to create will not be used to make couplings and therefore will not matter its definition. to do the couplings with axes and planes is not very practical and tends to set it aside for other more direct
2. create the cylinder representing the threaded part and a surface (or a thin extrusion) that will represent the support face of the screw; with this method the body of the threaded part and that of the support you use to make the couplings will always be equal for all types. This method is more practical using faces generally to make matings, but it requires greater attention in modeling.

if during the assembly phase you realize that instead of a hexagonal screw it is better to use a cylindrical head you just replace component and you will not lose any coupling.


for the hardly configurable commercial parts you can find a lot of material on traceparts