Automated Title Block and more

Question

Automated Title Block and more

theribeiro (Computer)

(OP)

19 Aug 20 12:15

Hello everyone ! my name is Andre. Im an IT student internshipping in a metal design factory working for the first time with Catia.
I'm working using Catia v5r26.

So here they have a custom title block someone made, and they use it for all the parts.
The thing is they have it in a CATdrawing, each time they need it they create a copy of the file and delete the previous part views and data. And they fill the gaps with the new information by hand.

I'm trying to find a way to have the custom title block in a macro or by someway that would be more easily acessible. And fill the gaps such as date, number part, material and Designer automatically (getting that information from the part itself).

1 - Would there be a way to "transfer" the custom title block they have into code ? or do i need to draw it all over again ? I don't have much experience creating tables and its not simple, it has different column and row width, an image...

2 - Can I get that automated filling of the gaps using only formulas ? or is macro necessary too ?

I've searched but haven't found a thing like this. However if you can send me links or something I appreciate :D

Thank you in advance, any help is amazing

André

ferdo (Mechanical) · Answer 1 · 2020-08-19 12:38:30

Google

Regards
Fernando

https://www.youtube.com/playlist?list=PL9mSHa4SOed...
https://www.youtube.com/playlist?list=PL9mSHa4SOed...

LWolf (Automotive) · Answer 2 · 2020-08-19 13:51:11

http://catiadoc.free.fr/online/driug_C2/driugbt010...
is the first search item...
but yes. My company has custom title-block script that draws everything...

regards,
LWolf

theribeiro (Computer) · Answer 3 · 2020-08-19 14:20:59

Thank you ferdo and Lwolf for the quick responses

I used their custom title block as a background view in Page Setup. Is it possible to get this into the code ?
I'm having problems also in filling the gaps

ferdo (Mechanical) · Answer 4 · 2020-08-19 14:33:30

Starting from a model, yes, it can be put in the code. You can find an example in CATIA installation folder, do a search for CATScript there (or title block, can't remember exactly)

Regards
Fernando

https://www.youtube.com/playlist?list=PL9mSHa4SOed...
https://www.youtube.com/playlist?list=PL9mSHa4SOed...

LWolf (Automotive) · Answer 5 · 2020-08-19 14:45:08

C:\Program Files\Dassault Systemes\B28\win_b64\VBScript\FrameTitleBlock

regards,
LWolf

theribeiro (Computer) · Answer 6 · 2020-08-19 15:02:36

Sorry, I wasn't clear. I mean my company's title block is what I'd like to convert to code not the default samples of Catia.
Is there an automatic way to do this ? or it has to be written ?

ferdo (Mechanical) · Answer 7 · 2020-08-19 15:09:15

To be written, no doubts.

Regards
Fernando

https://www.youtube.com/playlist?list=PL9mSHa4SOed...
https://www.youtube.com/playlist?list=PL9mSHa4SOed...

theribeiro (Computer) · Answer 8 · 2020-08-19 15:32:54

I saw on another thread, ferdo you wrote:
"In this case you can write on the drawing sheet a text in a specific point location. Put a point where you want to add text, take the coordinates and do it in a separate macro. Your text still can be added in the title block field, is not neccessary to open and edit the title block (I suppose is not a picture)."

I will try this instead.

ferdo (Mechanical) · Answer 9 · 2020-08-19 15:46:04

True, but first see if you don't have already some text boxes in those places. You can modify their value in a macro.

Regards
Fernando

https://www.youtube.com/playlist?list=PL9mSHa4SOed...
https://www.youtube.com/playlist?list=PL9mSHa4SOed...

theribeiro (Computer) · Answer 10 · 2020-08-20 07:32:50

I do have text boxes and I figured I can get to them using the "Insert Object Resolution" tool. Now changing their value I'm still looking for that. Can you point me in the right direction?

Set drawingDocument1 = CATIA.ActiveDocument

Set drawingSheets1 = drawingDocument1.Sheets

Set drawingSheet1 = drawingSheets1.Item("Sheet.1")

Set drawingViews1 = drawingSheet1.Views

Set drawingView1 = drawingViews1.Item("Background View")

Set drawingTexts1 = drawingView1.Texts

Set drawingText1 = drawingTexts1.Item("Text.82")

Little Cthulhu (Marine/Ocean) · Answer 11 · 2020-08-20 07:52:28

Quote:
Now changing their value I'm still looking for that.

CODE

Set drawingText1 = drawingTexts1.Item("Text.82")
drawingText1.Text = "My new text"

I'd say that you're going to have really hard time exploring those texts since they have auto-generated names. It means each time a text get pasted in a list it gets unique number as a suffix. So the same piece of a frame titleblock is going to have different names on different sheets.

theribeiro (Computer) · Answer 12 · 2020-08-20 08:20:30

Here's the titleblock.

Little Cthulhu I've tried your code and it ran but didnt change anything whatsoever.
I pretend to use this titleblock as a background view everytime we need it for a new product. Using page setup to get it. I've tested doing this and using the "Insert Object Resolution" tool and it gives the same output for each one of the text boxes as in the original. For exameple the text box with the 1 inside puts out object Text.79.

Can i change the names of the text boxes ?

[EDIT]- I now know I can change the name of the text boxes, would that facilitate the job ? still can't change the text inside it though.

theribeiro (Computer) · Answer 13 · 2020-08-20 10:00:08

i've got this :

CODE -->

Language="VBSCRIPT"
Sub CATMain()
CATIA.ActiveDocument.Selection.clear
Set drawingDocument1 = CATIA.ActiveDocument
Set selection1 = drawingDocument1.Selection
selection1.Search "CATDrwSearch.DrwText.TextString=*fillmaterial*,all"
Text1 = selection1.Count
'CATIA.ActiveDocument.Selection.clear
Text2 = "aluminium"
If  selection1.Count > 0 Then
selection1.Item(1).Value.Text = Text2
End If
CATIA.ActiveDocument.Selection.clear
End Sub

And it works but it goes by the content not the box. I dont manage to get the box selection working.

LWolf (Automotive) · Answer 14 · 2020-08-20 10:25:16

see Little Cthulhu last post

regards,
LWolf

theribeiro (Computer) · Answer 15 · 2020-08-20 10:46:55

I've tried this and it doesnt work. I'm sure there's something really obvious wrong with it.

CODE -->

Language="VBSCRIPT"

Sub CATMain()
CATIA.ActiveDocument.Selection.clear

Set drawingDocument1 = CATIA.ActiveDocument

Set drawingSheets1 = drawingDocument1.Sheets

Set drawingText1 = drawingTexts1.Item("Text_01")
drawingText1.Text = "My new text" 

End Sub

Little Cthulhu (Marine/Ocean) · Answer 16 · 2020-08-20 11:01:28

Always put Option Explicit in the first line of your every script. This way you're going to discover errors easier.

CODE

Option Explicit
Sub CATMain()
  Dim doc as DrawingDocument
  set doc = CATIA.ActiveDocument
  Dim view as DrawingView
  set view = doc.Sheets.ActiveSheet.Views.Item(1) ' 1 - background view, 2 - main view
  Dim txt as DrawingText
  Set txt = view.Texts.Item("Text_01")

  txt.Text = "My new text" 
End Sub

Little Cthulhu (Marine/Ocean) · Answer 17 · 2020-08-20 11:02:03

Always put Option Explicit in the first line of your every script. This way you're going to discover errors easier.

CODE

Option Explicit
Sub CATMain()
  Dim doc as DrawingDocument
  set doc = CATIA.ActiveDocument
  Dim view as DrawingView
  set view = doc.Sheets.ActiveSheet.Views.Item(2) ' 1 - main view, 2 - background view
  Dim txt as DrawingText
  Set txt = view.Texts.Item("Text_01")

  txt.Text = "My new text" 
End Sub

theribeiro (Computer) · Answer 18 · 2020-08-20 11:23:19

Didn't work, gave an error right in the:
Dim doc as DrawingDocument

LWolf (Automotive) · Answer 19 · 2020-08-20 11:41:02

actually, background view is View.Item(2)

regards,
LWolf

LWolf (Automotive) · Answer 20 · 2020-08-20 11:43:19

... but I cannot seem to identify a text-item by its' name reference "xxx", only by item number?...

regards,
LWolf

theribeiro (Computer) · Answer 21 · 2020-08-20 13:27:24

LWolf with the code I posted above I can get to the value of the text box, by searching it in the drawing and changing it to something else. What I'm not able to do is select the text box itself to change what's inside it. Till now with no success.
The number inside doesn't serve any purpose, merely to enumerate the boxes. The boxes names go like Text_01 ...

Little Cthulhu (Marine/Ocean) · Answer 22 · 2020-08-20 13:56:41

Quote:
actually, background view is View.Item(2)

Thanks for correcting.

Quote:
Didn't work, gave an error right in the:
Dim doc as DrawingDocument

What error? Post a screenshot.
More information saves time.

theribeiro (Computer) · Answer 23 · 2020-08-20 14:02:55

CODE -->


Option Explicit

Sub CATMain()


 Dim doc as DrawingDocument
 set doc = CATIA.ActiveDocument
 Dim view as DrawingView
 set view = doc.Sheets.ActiveSheet.Views.Item(2) ' 1 - main view, 2 - background view
 Dim txt as DrawingText
 Set txt = view.Texts.Item("Text_01")
 txt.Text = "My new text" 
End Sub

Sorry It's in portuguese, but it basically says Error in compilation, End of instruction missing

ferdo (Mechanical) · Answer 24 · 2020-08-20 14:31:41

You are using catvbs, you need to replace all As with 'As - check the documentation why, this code is working in CATScript

Regards
Fernando

https://www.youtube.com/playlist?list=PL9mSHa4SOed...
https://www.youtube.com/playlist?list=PL9mSHa4SOed...

theribeiro (Computer) · Answer 25 · 2020-08-20 14:45:47

CODE -->

Option Explicit

Sub CATMain()

Dim doc as DrawingDocument

set doc = CATIA.ActiveDocument

Dim view as DrawingView

set view = doc.Sheets.ActiveSheet.Views.Item(2) ' 1 - background view, 2 - main view

Dim txt as DrawingText

Set txt = view.Texts.Item("Text_01")

txt.Text = "My new text" 

End Sub

I've tested with CATScript too and it puts out another error :

It says Incorrect type : 'view.Texts.Item'

LucasC (Automotive) · Answer 26 · 2020-08-20 16:22:03

Here's a sample of my code for changing titleblock text boxes (in sheet background). This is used on a userform so some strings refer to clickable buttons or text boxes there.

CODE --> CATVBA

Dim DrawingDoc As DrawingDocument
Set DrawingDoc = CATIA.ActiveDocument

Dim TitleBlockTexts As DrawingTexts
Set TitleBlockTexts = DrawingDoc.sheets.ActiveSheet.views.Item("Background View").Texts

Dim Weight
Set Weight = TitleBlockTexts.GetItem("TitleBlock_Text_Estimated_Weight")

'.... code for other unrelated functions

If WeightApplyAll.Value = False Then 'disregard the If...Then I have an "apply to all sheets" toggle button on my userform
Set Weight = TitleBlockTexts.GetItem("TitleBlock_Text_Estimated_Weight")
Weight.Text = UCase(Title_Block.Weight_TB.Value) & " " & LCase(Weight_Unit_LBL)  '"Weight_Unit_LBL" is for a kg/g option on my userform
End If

Little Cthulhu (Marine/Ocean) · Answer 27 · 2020-08-20 17:46:36

See LucasC post, replace Item("") with GetIten("")

LWolf (Automotive) · Answer 28 · 2020-08-21 09:06:14

yupp, GetItem does the trick! thx

regards,
LWolf

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