I'm going to you because I have a problem with the control of the dimensions. Let me explain:
I am doing an internship at the end of my studies and I have to create a model of a reference part on which I will have to apply variable parameters according to customer requests. Unfortunately, from one customer to another, the same rating can be both driving and controlled. It all depends on the designer. And I have to plan for that.
A constraint of my tutor is that he would like that by pressing a simple button (the purpose of my project), the numbers entered are integrated into the model and at the end of a plan being made. So we should be able to choose beforehand which dimensions are piloting and which are piloted before pressing the launch button, but without going back to the sketch.
That is to say maybe find a way to tell Solidworks that I want these controlled dimensions and the other pilots, but I'm drying up ...
I would be you, I would look for the families of parts, you can control the dimensions of your parts easily. You can also check your dimensions using VBA (macro) as the coin families go through Excel.
Hello How do you plan to do this? By excel / by the equations page or small in-house software?
On the other hand, I don't see why it would depend on the designer for the same part, but more on the customer if he wants interior or exterior dimensions for example.
It also depends on the number of odds to be switched to pilot or not and also to avoid any overrating you need to find a simple way to deactivate and automatically activate the additional odds.
On the other hand, if your tutor asks you to do it via "a simple button", I would lean towards a software solution / VBA or c++. (you still have to know about it)
On the other hand, the "simple button" thermes is generally used by bosses or department heads who unfortunately don't know much about the software used, but I could be wrong;) (from my own experience)
I'm not saying that it's unfeasible but that it's not as "simple" as that.
I don't know, any manipulation would do but it's true that the VBA on Solidworks is quite complicated, and for my part completely unknown.
The problem is that the number of dimensions driven is around the same number for each part but is never the same and can vary depending on the customer.
Indeed I doubt the feasibility but my project depends on it so I have to find a solution to switch controlled -> driving or vice versa in a quick way and why not configured with Excel or VBA but I don't know the syntax that allows this ...
I tried to save a macro on solidworks when I switched from driver to driven but it doesn't display anything on the macro corresponding to this action
Macros227 I already have about 2000 configurations (including derivatives) that allow me to define the shape of my part in all places, so adding other derived configurations for the dimension driver would be infeasible....
I don't understand why you should turn off or on certain dimensions, we don't necessarily have the same dimensions depending on the designer but someone who takes an existing part is not going to have fun changing the origin of the dimensions, logically.
If I understood correctly, basically you have a hole on the left line side at 20 mm, you want to turn off this dimension to turn on the right dimension which is at 40 and you go from 40 to 50 for example. But why, why not change the rating from 20 to 10 ?
On this system you can make tables of equations with the sides to be modified, it's easy to access but a bit restrictive. Otherwise it's VBA you bring in a small table where you complete the odds you want to modify, but it's already a little more complicated.
Small "problem" on the VBA if you have ten different rooms you have to do 10 different programs, or else make sure that the height rating is in exactly the same place, example D2@Esquisse1@pièce, which can give Hauteur@EsquisseBrute@pièce.
Hello, you can change the state of a dimension (piloted/piloting) via a family of parts like any other sketch relations by the way.
To do this, you need to identify the name of the sketch relationship corresponding to the dimension (see in the list of sketch relationships) and then transfer it to the part family.
For example, for the first dimension of my sketch named D1@esquisse1 the corresponding sketch relationship name is Distance1@esquisse1.
To control this sketch relationship in the part family, it will be sufficient to note:
DriveWorksXpress enables assemblies from defined part libraries. But does it allow you to modify the dimensions inside a room and in addition to making them appear piloted that, I'm less sure.
Kind regards
PS: only the ultra-basic version is free, the PRO version is paid but if it's really useful then it's worth it.
Zozo_mp, DriveWorks technology allows for much more than joining library parts. It is possible to control dimensions, functions, colors, materials and much more.
DriveWorksXpress is quite simple, but completely free.
The two higher versions bring more features, including document automation, the ability to use online forms, 3D previews and integration with other software.
I finally found the solution using a macro I created. First of all, I made the choice to place ALL the dimensions in driven . And in the macro, I say that if (in Excel) the value of the dimension is filled in via Excel, then it becomes drivenState and takes this value. Otherwise, if the call number is NOT entered in Excel, the call number remains controlled.
I share this tip in case anyone stumbles upon a problem of this magnitude^^