Hello
We regularly work on files that are a bit large (20 / 25000kb) and during the drawing it is very complicated to carry out... A CUP!!
Display time> 10 minutes, or even impossible.
I work on HP Z4 G4 Workstation / 16GB RAM / Windows 10 pro
I did a try, after having made a "pack & go" of the file, to repatriate all the details in the same folder on the "C" disk...
Open: "complex assembly mode"
What solutions do you adopt to avoid having this type of problem?
We found a solution, an additional position at the design office and we start the cutting and make big shots on it so we start the cut and we come back 30 minutes later!
Unfortunately, this is the reality on large assemblies, it is complicated to make the drawings and in particular the cross-sectional views...
GLUPS!!
I hope this is not the only possible answer.... I used another similar software for 10 years to do the same job, and I didn't have this type of problem. When I look at the demos of SW 2019, I ask myself questions... How many KB is a complex assembly from?
For me, it's not the weight of the assembly that makes it heavy, but what makes it up.
I can have an assembly made of 4 other assemblies so little constraint but in each of these assemblies heavy parts like wire mesh with repetitions, sheet metal with multitude of holes or simply large numbers of parts or worse surface parts that cuts them don't like at all.
And this assembly, which is not heavy in weight 4 constraints and 4 references, is still very heavy to process for solidworks, especially when cutting.
On the other hand, complex assembly I forgot, I find it even slower to process. The opening is faster for sure but I find that the time saved during the opening is quickly lost in greater slowness so I open all in resolution. With assemblies of more than 10000 components sometimes hence the additional pc available ...
Thank you for these remarks.
I just ran ""performance evaluation" __> total number of components: 671 (?)
I ran on another PC, the cup spins, turns, spins but no convincing result.
We should give the whole result, the number of bodies is even more significant.
But, if the problem arises with only 671 components (even if there are, for example, screws repeated many times), I would rather see a problem with a component that is on the surface.
Okay, but we don't use parts that are created in the surface.
Excuse me
There are in the sub-assemblies parts in PRT from STP. and therefore in surface. I'll make some changes to see if that's the reason.
Hello
we also had a lot of problems with drawing (creation of sections / conversion to DWG....) on relatively heavy ASM files (4000 components / 7000 bodies / a hundred constraints).
After a wave of tests, it turned out that to save time on drawings, it was necessary to master the design from the creation of the parts , for example:
- No surface area
- No or very few external references
- No use of imported files (e.g. engine) but rather recreation of the model in "lite" version
- Limitation of configurations, use of display states instead
All this with the aim of reducing the size and resources required for the software to display/reconstruct each part or assembly.
For the record, on the same assembly, one raw as we designed it and the other with the modifications described in part above, the gains on the drawing were considerable: 70% time saved! (Creation of section / conversion to DWG).
Hello
In our company, we make HDPE tube lifting stations.
For a long time, I tried to make a cross-sectional view of only certain elements...
Visiativ found me a pretty good solution: use the configurations.
So since every part of my library that I would need to see in view of cutting, I have the following configurations:
And each assembly also has this same configuration list. Once configured, it works perfectly.
I hope this helps you
Kind regards
Hello
I proceed in this way and then I record this part outside the assembly. By making a part of the assembly and with this way of doing the part keeps a link with the assembly. If you edit a part in the assembly, the part you created from it will follow... So it's easier to make cuts of a part than of a large assembly.
Hello
I tried to reduce the files containing surface as much as possible, but the problem persists...
In addition, I use database elements (Bearings, Motorization) from step files and solved in part and therefore in surface.
2 points also surprise me when I want to create a cut:
1st: when I place my cup, and before validating, the view is placed correctly. But when I validate, the definition loops and searches indefinitely.
2d: if on the elevation view (corresponding to the desired section) I create a local section, it works...
In the future we will go for the solution used by Drix49 , but I am not convinced by the system and I have the impression that few people make plans with cross-sectional views.