Hello
I'm looking for how to put on a part the number of occurrences it has in an assembly.
The goal is to put only one screw in an assembly and say that it is present n times for the nomenclature to be correct.
This function existed in solidedge but I couldn't find it in solidworks.
Thank you for your answers
Hello
In fact, you would only want to put one in the assembly and then the bill of materials tells you that there are 20 for example??? If that's it; It seems to me that this is not possible. Unless you force it into the nomenclature.
Sorry as ditto @ ac cobra
no choice they have to put the screws
then it is possible to put them in a specific screw folder
and hide all or part of them.......... if you want
but they will appear in the nomenclature
which of + is via the auto constraints it goes super fast
a simple selection of the said screw and approach the hole it places itself
each CAD log has its own specific phylo
an advantage with SW is that you only count what is put in the assembly
@+ ;-)
Hello
it is possible to add a custom property on your part (e.g. "Quantity")
Then define its value: the number of entities (e.g. 20)
Then define this property as the one used for the quantity in the BOMs (drop-down list at the top right of the property definition window)
http://help.solidworks.com/2018/french/solidworks/sldworks/t_linking_a_custom_property_value_for_a_part.htm
Please note: this is suitable for parts that are specific to a particular assembly or that are always used in this quantity. The information is stored in the part file. It is of course possible to vary this property in a way that is specific to the configurations of the room.
For other cases, you will either have to copy the part file (to vary the quantity).
Or use virtual components (making them independent to have different quantities):
http://help.solidworks.com/2018/french/solidworks/sldworks/c_vc_virtual_components_overview.htm
Good luck!
so not so usable for the case of screws
which by definition are not specific to an assembly
it seems to me but several in theory
@+ ;-)
You might as well do a controlled repetition (it implies that the holes are made via the wizard for drilling and/or repetition) and you will be sure that the quantity indicated will be correct (don't forget that any value entered manually is potentially wrong).
To do this, a simple trick is to do a "Repeat by rotation" of the screw on itself (180° steps).
Disadvantage, risk of distorting the cdg (mass), but this can be negligible.
there is more than the desired quantity entered, it remains independent with each assembly...
In fact, today we put all the screws, washers and nuts using the repetitions or driven by the sketches. Indeed it is not very complicated and quite fast. But we work on large assemblies and these hundreds of screws, if not thousands, inevitably slow down our stations.
I found a trick that consists of putting the quantity on the component in the "Component reference" variable which is located in "Document Ownership". This variable can be brought back into the nomenclature and with a small multiplication formula the correct number of screws can be displayed. The disadvantage is that it will create as many lines and therefore as many marks for the same screw.
After so big an assembly,
there is the classic technique of creating a "Screws" folder at the end of the shaft,
Similarly, if there are repetitions, when we manage the screws, we always think about creating repetitions dedicated only to the screws (other than the repetition of components).
and to create a config in the ASM without (or a MEP-with-Screws),
or we will put the screws folder, and the screws repeats in the deleted state ...
(off-topic poll: how do you prefer to write CHC or CHc? me CHC)
I am also more inclined to create a specific folder and deactivate (deleted state) in the desired configuration its parts and associated repetitions.
Off-topic answer ;-): I'm also more CHC!
Another off-topic note: you know why SolidWorks names "remove " deactivating a part instead of just "deactivating". It is never easy to explain this term to novices! Because for me deleted is more synonymous with "Delete/delete" from SolidWorks.
Hello
Solidworks has improved its handling of large assemblies, do your general settings use the complex assemblies and large designs modes? (limits recalculations...)
Otherwise effectively manage a full configuration with all the screws a conf light without.
@Antho : "delete" comes from the fact, in my opinion, of deleting from the display (in connection with the display states), deleting being a permanent deletion. So no real inconsistency.
Another technique: using empty components, disadvantage the lack of visual in some cases.