You can already see the surface of the room but it takes all the surfaces of each room, and I would only like the surfaces that can be painted.
To calculate the amount of paint needed on a part or assembly.
Would it be possible to have the surface to be painted of a part or assembly directly on solidworks?
Hello
To achieve your goal, you need to proceed in two steps.
- You have to paint each surface individually (look at the mini-tutorial I proposed https://www.lynkoa.com/forum/conception-3d/rendu-couleur-des-assemblage-sur-solidworks?page=0#answer-1083308)
- You need to select the surface and activate the measure function, you will have the surface automatically.
These are the two ultra-basic methods, but my colleagues will hopefully give you other, more automatable solutions.
Kind regards
1 Like
Okay, thank you for the answer.
But yes, what I'm looking for is something automatic because it would be useful for a program that would take this data directly without having to enter anything.
Hello
It depends on what is called automatic because it will be necessary to designate at a given time the surface to be painted. It depends on how the volume is made, for example, if you make a cube and you want to paint only one side, well you can't use extrusion as it is, because you have to go through appearances because the dsplay nanager is of no use in your case.
This surely means being able to either designate the surface to be painted by hand (or by a code). Then with a macro that will launch the surface measurement and constitute a list with "N" characteristics put in a file that can be used in Excel.
Have you looked at the tutorial to realize the complexity of what you want to compare to ==> select the face ==> click on measure ==> put the information in a ??? linked to the room.
Kind regards
2 Likes
Hello;
Have you thought about Sensors?
http://help.solidworks.com/2020/French/SolidWorks/sldworks/c_Sensors_OH.htm
To be displayed directly in a Nomenclature?
2 Likes
Hello
As you can see as an example in my attachment, the part is welded, then painted and what I would like to have is only the surface of what is in red and not what is inside. In other words, the surfaces are visible to the naked eye, the outer surfaces. You see?
So the sensors are of no use to me except if they have a function that I don't know.
Yes, I am aware of the complexity of what I am asking for, but the development of a program would not be possible?
capture.png
Hello
Given the center of gravity symbol on the last capture, it is an assembly?
In this case, it is possible to create a part in the context, then with the " offset surface" function to copy all the faces of the same color (see offset them by 0.05mm to avoid display bugs), then it is enough to retrieve the surface variable of this part in the nomenclature.
The operation can be repeated for each color.
PS: the solution of @ZozoMP combined with @Maclane 's are the 1st that came to mind as well.
2 Likes
Yes, this is an assembly and there are a lot of components under the closing sheets, so the surface is not precise enough and would make us order way too much paint.
Is it possible to copy all the faces of the same color at once? Without having to select them all?
Hello @l.manceau
"Is it possible to copy all the faces of the same color at once? Without having to select them all?" you don't have to try
Hello
It seems possible to me by macro, here is one that should be able to serve as a starting point, it is probably to be adapted to your needs:
Option Explicit
Sub main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim Assembly As SldWorks.ModelDoc2
Dim myAssy As SldWorks.AssemblyDoc
Dim myComps As Variant
Dim myCmp As Component2
Dim swSelMgr As SldWorks.SelectionMgr
Dim swSelData As SldWorks.SelectData
Dim swPart As SldWorks.PartDoc
Dim swBody As SldWorks.Body2
Dim swFace As SldWorks.Face
Dim swEnt As SldWorks.Entity
Dim bRet As Boolean
Dim vBodies As Variant
Dim vMatProp As Variant
Dim mySurface As Double
Dim myColor As String
Dim mySearchColor As String
Dim i As Long
Dim ninfo As Long
Set swApp = CreateObject("SldWorks.Application")
Set Assembly = swApp.ActiveDoc
Set myAssy = Assembly
mySurface = 0
myColor = ""
myComps = myAssy.GetComponents(False)
For i = 0 To UBound(myComps)
Set myCmp = myComps(i)
bRet = myCmp.Select2(False, 0)
bRet = myAssy.EditPart2(True, True, ninfo)
Set swModel = myAssy.GetEditTarget
Set swPart = swModel
swModel.ClearSelection2 True
Set swSelMgr = swModel.SelectionManager
Set swSelData = swSelMgr.CreateSelectData
vBodies = swPart.GetBodies2(swAllBodies, True)
Set swBody = vBodies(0)
Set swFace = swBody.GetFirstFace
'C'est ici que l'on définit la couleur à chercher
mySearchColor = "[255, 0, 0]" 'rouge
'mySearchColor = "[0, 255, 0]" 'vert
'mySearchColor = "[0, 255, 255]" 'cyan
Do While Not swFace Is Nothing
vMatProp = swFace.MaterialPropertyValues
If Not IsEmpty(vMatProp) Then
myColor = "[" & vMatProp(0) * 255# & ", " & vMatProp(1) * 255# & ", " & vMatProp(2) * 255# & "]"
If myColor = mySearchColor Then
Set swEnt = swFace
bRet = swEnt.Select4(True, swSelData)
mySurface = mySurface + swFace.GetArea
End If
End If
Set swFace = swFace.GetNextFace
Loop
myAssy.EditAssembly
Next i
Debug.Print ""
Debug.Print "Surface totale de couleur " & mySearchColor & " : " & mySurface
End Sub
Kind regards
1 Like