Hello
does anyone have a FORSTER profile base in SW by any chance?
I would like to avoid doing hours of conversions for nothing ;-)
Charged with revenge
Hello Francis
Obviously they only put DWG (RHAaaaaaaa!) and nothing at PartComunity.
So unless you have a mass conversion mill, it sucks.
Look at MyCadtools full compatible with SW or a colleague's macro.
Kind regards
2 Likes
Hello Francis, hello Zozo_mp
I applied to 3DPartsCatalog to add the Forster library
They tell me it will happen on 11/2021. On the other hand it will remain in dwg format
Cdlt
3 Likes
thank you zozo_mp for your answer but I haven't found enough to do a mass import....
acombier, I have the FORSTER library in DWG but as it is it is not usable in the library of soldered elements? thank you anyway
Anyone else have an idea?
Hello
I don't know the Forster profiles. Are there a lot of them? How many families can we regroup ?
If the profiles are close to each other, if there are only a few values that evolve, it is possible to control the profiles via an EXCEL file, so it is easy and quick to make a family of parts that you can feed as you go along with your projects.
May the force be with you.
4 Likes
hello OBI WAN
To your questions answer I can: there are more than 100 profiles. group them by 4 families it is possible
can you help me because I don't know at all how to manage them by EXCEL (each profile is different but quite similar anyway)
I'm on the dark side of the project ;-)
1 Like
Hello
Why not use Batchconverter which does this very well https://www.youtube.com/watch?v=wJeSg5cO06s
@jmsavoyat know quite a lot about the subject https://help.visiativ.com/mycadtools/2019/fr/BatchConverter.html
Kind regards
1 Like
can you post 2 or 3 profile examples of the same family.
may the force be with you.
For me they are different families because they are not the same geometries.
When I pale from the same family it is for example a UPE 100 and UPE 120.
I attach an excel file UPE part family for example, to see the structure.
It's the same principle as the family of parts.
make a profile, name the dimensions (to make it easier), make the family of parts, save format. SLDFP.. and place it in the folder where your libraries are already located.
The big advantage is that when you go from an IPE 100 to an IPE 120 (for example) it's a sketch that evolves, you don't change the body so the hook point doesn't change.
I am at your disposal
may the force be with you.
upe.sldlfp
1 Like
Hello @
I would like to say that the dimensions are not necessary for the profiled sections, they are only used to
- make an automatic description (this is not the case because these profiles have standardized descriptions independent of the dimensions of the section).
- or to constrain the sketch for manual modification (which is not an option),
It will be necessary
- Insert the dxf as a part sketch
- Add insertion points if necessary.
- Fill in a description
- Save as sldlfp while selecting the sketch.
(Indeed it's hundreds of profiles, do better as obi wan said and enrich the library as you go,)
1 Like
OBI WAN
great sage that you are... so there is no possibility of grouping by family because all profiles are different :-(
well I think I'm good at drawing them 1 by 1..
Thank you anyway for your help (and zoo_mp's) I'll try with Batch Converter but without any conviction
thank you Lynk for the tutorial ;-)
I managed to make a part but I have problems adding insertion points in a curve (middle point for example) yet I proceed as in the training, it works on a rounded angle at 90° but not a curve at 180°I really suck!! .....
Can you make a screen print,
by doing control and selecting the line before the curve and the one after it works on a 90° but that's it
capture_decran_2021-10-15_121352.png
It is possible to add as many construction lines as needed (after fixing the entities ctrl+a fix, to keep the shape of the section).
0001.png
Hello @francis_2
What do you think of batchconverter it would be a hundred times easier, especially over time. (see my post published a little earlier
I guess you're being asked to spend more time on the already complicated design without wasting time converting DWG files.
For the quality and time not wasted when you know that a design office costs between 50 and 90 € per hour at the cost charged. The gross monthly minimum wage (based on 35 hours) is €1,589.47 ).
Comparing these skilled labor costs to that of Batchconverter is peanuts for the latter, in any case it's worth the cost to look at, not to mention that the tool will be useful for other things, especially the doc.
Kind regards
1 Like
Hello
Although I'm not sure that the time saved is that important since the longest part is not to transform these dwgs into sldlfps but it is probably to rework the sketches obtained so that they are "usable" in SW, here is an example of a macro allowing you to list the dwg files present in a folder in order to convert them into sldlfp files.
' Attention: ne pas oublier d'ajouter la référence Microsoft Shell Controls And Automation
Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim boolstatus As Boolean
Dim swSheetWidth As Double
Dim swSheetHeight As Double
Dim swFeature As Feature
Dim myFeature As Feature
Dim theFeature As Feature
Dim PartModel As String
Dim DWGName As String
Dim SldlfpName As String
Dim featCount As Long
Dim featName As String
Sub main()
Set swApp = CreateObject("SldWorks.Application")
defaultTemplate = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)
PartModel = defaultTemplate
'Stop
Dim Path As String
Dim Folder As Object
Dim objFolder As Folder
Dim objShell As Shell
Set objShell = New Shell
Set objFolder = objShell.BrowseForFolder(0, "Veuillez sélectionner le dossier des fichiers DWG à traiter.", 0, 0)
If (Not objFolder Is Nothing) Then
myPath = objFolder.Self.Path
Else
MsgBox "Erreur"
Exit Sub
End If
'Stop
myFile = Dir(myPath & "\*.dwg")
Do While myFile <> ""
DWGName = myPath & "\" & myFile
SldlfpName = Replace(DWGName, ".dwg", ".sldlfp")
swSheetWidth = 0
swSheetHeight = 0
Set swModel = swApp.NewDocument(PartModel, 0, swSheetWidth, swSheetHeight)
Set swFeature = swModel.FirstFeature
Do While Not swFeature Is Nothing
FeatureTypeName = swFeature.GetTypeName2()
If FeatureTypeName = "RefPlane" Then
FeatureName = swFeature.Name
Exit Do
End If
Set swFeature = swFeature.GetNextFeature()
Loop
boolstatus = swModel.Extension.SelectByID2(FeatureName, "PLANE", 0, 0, 0, False, 0, Nothing, 0)
Set myFeature = swModel.FeatureManager.InsertDwgOrDxfFile(DWGName)
boolstatus = swModel.ForceRebuild3(True)
featCount = swModel.GetFeatureCount
Set theFeature = swModel.FeatureByPositionReverse(0)
If Not theFeature Is Nothing Then
featName = theFeature.Name
End If
boolstatus = swModel.Extension.SelectByID2(featName, "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
Dim swErrors As Long
Dim swWarnings As Long
boolstatus = swModel.SaveAs(SldlfpName)
swModel.GraphicsRedraw2
swApp.CloseAllDocuments (True)
myFile = Dir()
Loop
End Sub
Kind regards
5 Likes
Hello @d.roger
For discussion ;-)
[HS ON]
You say ""it's probably to rework the sketches obtained so that they are "usable" in SW,"""
Sketches should always be good since all these types of profiles are made by extrusion or wire drawing, which means that the dies mounted on the machines are equal to the finished profile.
Or the DWG files provided by FORSTER are inaccurate, which would be surprising given what competitors do.
Can you enlighten us on your point of view out of pure curiosity ;-) ;-) ;-) Thank you!
[HS /OFF]
@Zozo_mp what @d. Roger meant I think is that in any case the sketch will have to be taken over because there must be no line that is superimposed and one that the sketch includes a single closed profile, it is also necessary to add the insertion points and for this possibly go through construction lines
3 Likes