Retrieving the properties of a welded construction body on a plane

2D plans Labelling system
1

Hi all

I need help with methodology.

I am used to working with Inventor which is very easy to use as far as drawings and bills of materials are concerned. We have recently been working with Solidworks 2024 SP5 in our company.

We wanted to experiment with the welded construction module. This one is pretty nice to use... Except for the plans. At least, with our current methodology.

Let me explain:

Our company designs and manufactures electro-hydraulic lift tables. So we are in boilermaking/metallurgy. We have all the resources at home: scrap yard, machine shop, assembly/welding, hydro-electricity. , painting/finishing, packaging/shipping. We have total control of all our raw materials and all our products (including cylinders).

This structure requires us to make detailed plans of our mechanically welded assemblies. For example, I have a first level of " equipped " sub-assembly whose plan contains a bill of materials with ALL the parts of the latter (mechanically welded or not) that we then enter into our ERP.

In this nomenclature, our table consists of information in the following order: Coordinate system / Machining plan number / Quantity / Designation / Length / Width / Material / Manufacturing method / ERP code.

If a part contains machining (milling/drilling), it will have a particular manufacturing method so that the plan can go directly to the right place in the workshop. So it also has a machining plan number, which corresponds to the Drawing Number/Coordinate System (For example, if I have a chassis plan that has the number 01 and my machined part has the coordinate system 12, the machining plan number will be 01/12)

When the manufacturing methods and the machining plan numbers are defined, we make the detail drawings that we call " Flow Plans". Each machined part has its own unique plan with its views and dimensioning. This allows us to correctly sort our plan folder according to the workshop destination.

The problem I have is that when I want to do this methodology with welded construction mixed with assembly, I have to fill in the properties of each part. For welded construction, these are the properties of the cutlist. I would have to be able to retrieve these properties in my plan, because I have a specific cartridge that differentiates between a flow plan and a timeline. Today, I have not found any way to be able to recover these body properties from the welded construction. It's a shame, because the welded construction is rather well done and allows you to make welded mechanics very quickly, but suddenly the time saved in 3D is largely wasted in 2D since I have to fill all my cartridge by hand via annotations, piece by piece, sheet by sheet (and when you have large sets, it quickly becomes very, very long).

My question is: Is there a way to recover these properties? Via a macro or a myCAD tool for example? Or maybe a feature I don't know about on Solidworks?

You will find attached an unfinished sample plan.

24-1011-06-FALSE CHÂSSIS.pdf (247.8 KB)

Thank you in advance.

1 Like
2

Hello rbessonnet and welcome to the forum,
Well all this information can be done directly on the bodies of your spare parts list, by right-clicking on each body ...
I can't take a screenshot because my pc is being processed.
… Keep us informed, @+.
AR.

3

Hello
Normally in the options of the inserted table, you have to check " Detailed list of welded parts".
image
As long as the properties used in the list of welded parts are the same as those of the parts files, it will fill in the right columns.

2 Likes
4

Hello Cyril_f,
I agree with you, as long as the bodies of the list of welded parts are well filled in with their information in their properties.
@+.
AR

1 Like
5

Hello AR, hello Cyril,

Obviously my problem is not very clear:

When I right-click on the list of welded parts in my welded build, I have access to properties that I can enter by body of the cutlist.

I would like to be able to retrieve these properties via an annotation when I make the " flow plan". But when I want to make the link, the software only offers me to select the file part of the welded construction, but not the bodies of this file.

6

Hello again rbessonnet,
So if you want to retrieve the properties of your welded parts list, then select your BOM and you save it in excel either in MEP or 3D, it should do it ...
@+.
AR.

7

Hello

Indeed, misunderstood the request.
So it is possible to recover the properties of the body.
Just link the note like this:
image
And then to recover the different desired properties.
For example, if you edit the text, the mapping is done as follows: $PRPWLD:" Prop "

4 Likes
8

Cyril, indeed I can link an annotation with this property! So I need to insert my soldered build body and then create an annotation and go and fetch the property or write it manually.

I may be asking too much, but obviously I can only put this property if a part of the welded construction is already inserted in the plan. But what if I want to integrate this into my blank basemap (document template) when I make a file > new and create a new drawing?

In any case, it's already a good start and it limits the damage if I have to change the properties of a part when I'm in the middle of drawing it.

9

There is the possibility to save this kind of annotation as favorites or even as an annotation library.
Just like a piece of a library then drag your annotation from the right pane (design library) onto your plan.
Method:
Create your annotation, select it, then click 1 to create the style and name it, then click 2 to save it to the design library.
image

Other topics for annotations:
Example here:
image
For the method see this topic:
https://forum.mycad.visiativ.com/t/bibliotheque-dannotations/95630/7?locale=fr&lang=fr
Or this video:

3 Likes
10

Name MEP part
'In the 3D part / List of welded parts / right click properties: Fill in the description " PERSONAL "
'Update the list of welded parts
'In a welded part plan, click on the part to be named
'Launch the macro to have your name written


Sub main()
Dim swApp As SldWorks.SldWorks
Dim myNote As Object
Dim swModel As SldWorks.ModelDoc2

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc

If swModel.GetType <> 3 Then Exit Sub '1 = pièce, 2 = assemblage, 3 = plan
Set myNote = swModel.InsertNote("$PRPWLD:""QUANTITY""x $PRPWLD:""PERSO""") 'Si pièce renommée en PERSO
Set myAnnotation = myNote.GetAnnotation()
longstatus = myAnnotation.SetLeader3(swLeaderStyle_e.swBENT, 0, True, False, False, False)

End Sub
2 Likes
11

I didn't know you could do that. Thank you for the tips, it will be very useful to me :slight_smile:

1 Like