Best practices in SolidWorks?

3D Design Volume Model
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Hello

If anyone can help me with SolidWorks, they will be welcome ;-)

What is the right procedure to follow to obtain files (sldasm or sldprt) that are stable or "clean" and that do not require reconstruction when re-opened on another workstation in the same or higher version of SolidWorks?

Are there any precautions to take when designing a part in SolidWorks?

Are there any recommendations for designing in an assembly file with SolidWorks?

Is there a command that thoroughly cleans the SolidWorks file(s)?

I need your feedback to support my opinion about SolidWorks.

Thank you in advance, for your answers.

Stéphane.

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Hello

There are many questions in your message, each of which deserves more than several answers
In order

1°) """What is the right procedure to follow to obtain files (sldasm or sldprt) that are stable or "clean" and that do not require reconstruction.

Answer: For parts (PArts) All files are stable and do not require reconstruction. On the other hand, if you modify a part and you do not update the ASM at the same time, when you open the ASM you will get a message telling you that you have a part in a previous state and asking you if you want to update it.

2°) "" when they are re-opened on another workstation in the same version or higher of SolidWorks? ""

Answer: whatever the position if you are in the same version you open without any PB the . You should know that there is backward compatibility. In other words, you can open all files from previous versions with the 2017 or 2018 version. On the other hand, no backward compatibility, with a 2017 version or lower you cannot open a 2018 (or a 2017 with a 2015 version). Although there are possible workarounds with certain limitations. All software is in this case: because a new function is unknown from previous versions, etc...

3°) """ Are there any precautions to be taken when designing a part in SolidWorks?  Are there any recommendations for designing in an assembly file with SolidWorks?

Answer: difficult to answer because the software has nothing to do with it if you design in a sober and intelligent way or like a pig with sketches and extrusions in all directions.  For an assembly of 10 parts I don't see what the problem would be, on the other hand for 1000 parts or more it is better to have a method by sub-assemblies, etc.... Here too, it is a question of the design of the person and the software has nothing to do with it. We frequently have discussions on the subject and each company, depending on the constraints of its business, adopts different strategies.

For deep cleaning it does not exist and in no software except WINDAUBE and DBMS.
 

I know and I have used 3 softwares: Inventor, PTC and Solidworks and the functionalities are pretty much identical on the other hand: I fired Inventor because for the static R.A.S but  for the kinematics it didn't work at all (a real m....) . I've been using SolidWorks for 10 years and I don't know many flaws (well, only one! but hey, just be careful).

In your choice you have to take into account the community which must be very active: I gave up PTC (and inventor too) for this reason at the time.

My little friends will complete :-)

Kind regards

EDIT: correction error between ascending and descending (sorry)

 

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Very good ZOZO remarks! On the other hand, what is the "ONLY" defect you have noticed on SolidWorks? Because I actually think like you that it's a software above the rest but there are SEVERAL flaws anyway :-)

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Hello Ronathan.

I must specify that this defect only appears when you do kinematics and move the parts copiously in the assembly (the ASM always makes more than 100 parts in my assemblies). In the design and for a relatively complex movement, it is necessary to check that there is no collision or that the trajectory of this or that part or of all the moving parts corresponds to what you want. So, we move the pieces with the mouse.

If you do, it crashes for a very long time. This is an AMHA problem is due to the fact that SW does not dynamically manage the memory of the computer or its internal variables which are not managed correctly. After a while it saturates even with a powerful machine like mine, even if all the memory is not used.

So, to get around the problem, you need to:

1°) Do the automatic backup systematically, but above all do it with a long delay between automatic backups (more than half an hour). I noticed that if you do certain operations at the time when the auto backup is done, it goes bananas.

2°) make a manual backup frequently to avoid losing the latest edits. This does not prevent the crash, but avoids howling wolf and cursing .........

3°) and above all close SW and restart it at least once an hour. This has the effect of resetting SW's memory to zero.

Note that when I'm not doing cinematics, I don't have the PB and even if I don't have too many parts or big assemblies open at the same time.

Note that this does not prevent me from working several hours a day without PB once these little tricks are respected.

Sincerely, and good sunshine :-)

 

Edit: Errata

 

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Hello

As Zozo said, The most important point is a clean build.
Cutting Solidworks completely from time to time does him a world of good, too.

If you create files with configurations, I recommend that you rebuild them all (Crtl+Shift+B) before saving your file and closing it. This will save you time when you open the part in an assembly, but it will increase the weight of the part.

To save reconstruction time in complex parts files you can use the block bar in the construction tree. Beware anyway because sometimes she does more harm than good.

To clean a file you can do a save under and overwrite the original file, it seems that this cleans up the file code a little.

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Thank you Zozo_mp , ronathan and  Pierre S.

I understand that SOLIDWORKS allows the freedom to design as desired,

And that to answer my questions, it requires an inventory of the design before deciding on the need for a methodology or not depending on the final quality of the 3D analyzed... which could impact the use of the final model.

2 new questions arise, then:

  • Without a training layer with recommendations to the designer, the 3D data exposes the design office to possible performance problems in its assemblies, I think correctly?
  • In the same way, that a good organization of the assembly structure is necessary to optimize the waiting times for the reconstruction, too?
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yes and... Yes for my part, everyone has to work with the same logic so that the openings are faster and that it is easier to find your way around if a modification is made by a delta character I think.

Cdt

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This requires a cross-functional  methodology...

Common to all trades for good practices starting at first.

Did I understand @G correctly? 

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+1 with the others so no need to say it again.

If you start with a brand new SolidWorks, make a personal folder to store all your models (parts, MEP, Materials, profile.....) it avoids typing the default infinite tree structure of SW and easier to transfer to another PC. (just to transfer the parameters from one station to another)

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Hello

Pierre S, how does the blocking  bar sometimes wreak more havoc?

Because we use it quite often, well my colleague especially.

So what are the disadvantages of this bar?

CDT.

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For my part, the big disadvantage is that as long as it is activated, you can't modify the room from the plan... After personally I have never had too many problems except that sometimes when you want to disable it, there is a bug that removes the blocking but the functions remain inaccessible. you then have to save, close the software and then re-open everything and everything goes back to normal (PS: I'm on solid 2015 SP5... sniff)

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The locking bar is especially useful for PRTs with heavy reconstruction, moreover you don't have to put it on the entire shaft.

(this requires a construction with anticipation... but can be very useful in some cases where you want to make modifications, adjustments)

Example: chassis with several tens of hundreds of function lines, part with "death" repeats, part with propeller sweep, etc...

With this we find the usual "food perf" functions of Solidworks, to which is added the use wrongly and through "External References" (but there are other ways to lighten the calculation-reconstruction...)

What is good is to know enough about the software to know how it has evolved, some functions, or function approach are not the original one, And very often a simple use with the "original methodology/philosophy" of the software is often the best, most stable, more reliable, etc...

Some examples:

1- Chassis construction, the default, the folders are not renamed, because the calculation/information of the table is not done there

2- Move Body, the "absolute" default is the basic function, move it constrained is an addition that remains buggy and unstable if used too much (bug for so many years... and not yet corrected)

3- The correct display of display filters, too often people (school outings, outdoors) use it incorrectly, maybe because they didn't understand how to use it correctly, or maybe because of a training that didn't talk about it correctly). I prefer to follow the basic philosophy of the software, which allows you to use level 1 filters, but also gives access to level 2 filters!

The display filters also make it possible to no longer have in the 3d the black line that passes through the models that represents the threads, but rather to have a representative texture that does not pass through the models!

Note the texture bug when you activate the cut, so to check the threads, tips to cut without validated does not bug, otherwise temporarily go over the line that crosses the models, and put yourself in orthogonal view (flat view)

4- Also over time, and the different versions of SW, the configuration of the DOT seems to have varied, or according to the companies badly modified... (that's a real pain...)

5- The calculated properties (mass, volume, area, density, etc...) are always put "in the config" and especially not "in the general".
As a reminder, in the first philosophy of Solidworks, a property is either in the general or in the config, not both at the same time (or else it's that we are aware of the behavior in the nomenclatures)

Example: display color of the planes, units, number after the decimal point in 3D (I prefer to work with non-truncated dimensions), display filter settings, setting of default configs (functions/constraints not removed), and the famous lighting adjustment! when you put the "orange" or the "white" of the color palette, does it appear like that in the 3D???

I had written a subject (big block) that talked a little about all this...

To come back to the question, in a 3D library, generally we use the file lock by windows, and in the part families, it is on the contrary preferable not to rebuild certain types of parts, because this allows to have a file of only a few kilos/mega, rather than several hundred...

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PS1: I also forgot in good practice, there is the way to put "correctly" constraints, so as not to overconstrain...

Unfortunately bad methods seem to be the most widespread (around me and my region), which means that simple assemblies of just a few pieces fall into carraffes...

there is also the principle of the "right reference" with the exercise A+B+C: Pièce_Fabriquée + Washer + Nut...

Example of a bad constraint :

bad constraint: coaxial / coincident / coaxial (the famous double-coaxial...)

bad constraint: coaxial / coincident / coincident (the famous coincident instead of a parallel...)

Good stress: coaxial / coincident / parallel

 

PS2: and also the principle of "judiciously" putting the origin in a PRT, or an ASM

PS3: and the principle of keeping the plane in front, as a major-shot/major-view of the PRT or ASM. And also keep the top planes in top planes, and in the ASMs, generally (except for the management of a particular origin) put the top plane as a ground plane...

example: in a new ASM, I insert a chassis made by someone else, I put it down, but it ends up on a side side...

The same goes for the library pieces, I insert a mannequin, it ends up upside down...

Another example in a drawing : I want to put a front view of my machine, I choose "front view" and boom, the machine is seen from below...

the choice of origin, plans... etc... All this is done with the principle of anticipation.

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PS4: "Under-Constrained" assemblies (with minuses, even for screws)

Apart from the case of movement studies, and hand movement, an ASM must not have a "- (minus)", it's like for sketches...

PS5: sketch under constraint (I prefer to even do it until the construction line, no blue in a sketch, except in special and wanted cases)

PS6: CAD library created and stored with the CAD language (filename), not that of an ERP, and with good subfolders.

Generally there are 2 basic structures that coexist together, a folder with the generic elements (with a good name, generic description...),

and one with the non-generic cad "named articles", associated with a manufacturer (example filename: Frabicant - Reference)

Always choose a manufacturer (for storage, naming), rather than a reseller!

PS7: a reference on its own means absolutely nothing, first we say from whom we take the component, then the reference.

PS8: then comes the management of unique identifants for a library, and the calculation of nomenclatures...

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Hello@Olivier42

I don't understand why you say that, if you could explain it, I'm interested.

(Example bad stress : coaxial / coincident / coaxial (the famous double-coaxial...)

Personally I do coaxial coaxial

Maybe I don't understand where the pb is since I don't have a problem.

On the other hand, I can give you examples of constraints that are sure to make a mess of complex assemblies :-)

I would ask you another question about how to have a positioning reference between several parts in an ASM.

Plush

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Zozo,

Of course we can give a whole bunch of examples of complicated constraints that are difficult to apprehend, as we can also give a lot of "bug zone" in solidworks (which was the case at the beginning of the subject, but I didn't want to intervene there)

the more parts you add, and the more you mix with the configs in the ASM (for the position, or other), the more you notice that the "constraint solver" falls apart because of the over-constraint...

I have a recent example, where I wanted to enclose a simple chassis in an ASM, put it first, and refix the origins correctly (front plane, top plane, etc...)

And here is the tree (I looked at how it was made "double coaxial" and other joys) and yet there are no more constraints with level 1, nor symmetry or plane-middle, nothing but "double-coaxial" (see screenshot)

As a result, it is impossible to "turn" the group of parts to re-align it correctly, this ASM is a bag of knots with only about ten parts...

a more telling example to put a part at the origin of an ASM, without going through "fix", we will put

plan-to-face on plan-face,

top-on-top-plane

Straight plane on straight plane

so it's not "good", it's better to put :

Front-plan on face-plan

top-on-top-plane

Origin on Right-Plane

or we can also (but this is another level of anticipation): 

top-on-top-plane

Origin on plan-face

Origin on Right-Plane

Straight plane parallels on straight plane

That way, if during the design process, you want to turn the piece, you can easily.

 

The A+B+C exercise is very telling, but not easy to explain like that, because it allows a gain in modifying, repositioning, transforming-adding sub-asm, or decomposing them.


capture.png
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ha!

OK @Olivier  I understood what you meant with your example, very interesting.

(origin on plan-face

Origin on Right-Plane

parallel to straight plan)

 

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@Olivier42: "level of anticipation"
I've noticed that this is the key to the problem and the hardest thing to get across. We are faced with a short-term reasoning for this kind of operation that makes us go for the simplest. I managed to get a screw, an axis to be correctly constrained (concentric, aligned, parallel), the notion of isostatism being, fortunately, known.
I'm going to have more trouble with your
"Shot-above-above-plan
Origin on plan-face
Origin on Right-Plane
Straight plane parallel to straight plane"

We can say that we are lucky to work with SW, which, at worst, when you drop the first part in an asm, fixes it in an "intelligent" way by default, with Inventor, the part stays where you let it go in the position where it is (i.e. really any way).

 

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It's nice that there are still "a few people" who work not too badly, or who try...

What hurts my heart is when I see files (at my work, or in the forums) where people use the SW display filters totally against the grain... yet it is part of his basic philosophy...

Reminder: everything that is construction is hidden, i.e. everything that is minor (axis, point, plan, sketch, sketch even in a PRT-Const-Soudé!)

and then you need the right display filter settings of course in the PRT, then in the ASM, then in the DRW...

this allows you to keep the major axes, or major planes, in level 1 filter, and to do other wonderful, fast, practical, and useful things in CAD!!

Question: Why redraw a dotted line of a door opening on a plan every time? when you can do it in "1 click"???

 

yet we learn to anticipate by being "lazy" and wanting to do as little as possible...

The top plane as a ground plane, it's very useful for machines, it allows you to know immediately an elevation, to put all the machines constrained by their "basic plans",

Using the basic plans instead of the geometry is very important too, so that in case of modification, we don't break anything, no constraint that jumps...

another example: in the construction phase, trial and error, with a multi-level ASM, several hundred files... several hundred constraints.

I have to restructure the ASM, reorder, create sub-ASMs, break down some of them...

With the wrong method, the user has set 500 constraints at the beginning, and will have to (example) redo 200 constraints to get the final result...

with the right method (constraint A+B+C...) the user has set 500 constraints at the beginning, and will have to do only 30 more to get the final result!

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PS9: you can put a knurled appearance "without going through Realview" (because it minimizes the performance in large assemblies) i.e. the old fashioned way, the menu has changed a bit of location but it's possible!

PS10: no need for third-party tools ! very often the functions already exist in Solidworks, and are sufficient for the desired need: bill of materials, layer management, property-tab, center of gravity, task scheduler, etc...

in SW you can still place a part in any way in an ASM.

for those who want to read my old "paved" topic (among other things, it allows to show/explain to people that EPDM can have other ways of being installed, not like the one "that we are sold indiscriminately", it's by digging into the settings and possibilities of EPDM that we realize what we are doing American programmers (even if sometimes some terms differ from Solidworks, due to the "computer scientist" vision) which allows to "unlock a part (only) of the SolidWorks features, it's always better than being limited to 98% in the use of CAD software.