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| Forum Highlight: CATIA V6 |
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SCOTTHAZEL
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| 01 Dec 2005 06:47 PM |
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Hello everyone. Is anyone familiar with the import button under the Formula function? I’ve got several dozen boxes in an excel document that I want as parameters in a .part. They are of mixed type. Some are in inches (in) and some are angular (deg). There is even one that is text. Every time I try the import, they all come in as text? There must be a way to import from excel and keep the original type. Anyone got any ideas?
Scott
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Scott |
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COE-FORUM-USER
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| 02 Dec 2005 02:53 AM |
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This works in R14:
(as csv, but should be columns in excel)
a, 3.4,, Comment 1
b, A test string,,
c, 5mm,,
d, 5deg,,
e, TRUE,, Comment 2
f, 45m,,
g, 2, a/23, Another comment
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BPRASAD
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| 02 Dec 2005 10:04 AM |
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What Scott did is correct. Make sure... in excell spreadsheet ...
The first column contains the parameter_name
Make sure the second column contains the corresponding parameter_value with its variable_type specified in (bracket)
The third column contains a "relation or formulae" you want to import. |
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Brian Prasad
COE-DPC/KBE Chairperson |
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COE-FORUM-USER
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| 13 Feb 2006 08:34 PM |
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hello...do u know how to link spread sheet to assembly drawing which when u up-to-date on spread sheet@bill of material,in assembly drawing also up-to-date automatically..if u know,plz help me...
thanks... |
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BPRASAD
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| 16 Feb 2006 05:17 PM |
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I am assuming your assembly drawing is associative to your 3D assembly -- which you have created.
If not the best way, to update your assembly drawing, is to make your drawing dependent on the 3D assembly geometry -- you have originally created.
Within the above 3D assembly, I suppose you may have linked several CATParts.
You can control the geometry of each CATPart(s) in the above 3D assembly, if you need to, through a series of Excel Spreadsheets via (Design Table feature of CATIA V5). You can link as many Excel Spreadsheets to each and every CATPart(s), as you may deem necessary. The process of linking the two (Excel Sheet to a CATPart) is described earlier on this thread or you can look into the CATIA HELP document.
If you do all of the above, you would be able to control your assembly drawings. You may have to manually update the drawing views every time when the associated values in the excel spreadsheet are changed.
Hope this helps.. |
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Brian Prasad
COE-DPC/KBE Chairperson |
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COE-FORUM-USER
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| 16 Feb 2006 07:06 PM |
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I tried as specified by bprasad to create a parameter of length using an excel file and importing it into a part file. However I can't get the second column to specify the parameter “type”; it won't come in as a length it comes in as a string. I tried all forms of brackets and parenthesis. Can anyone help or specify if I am doing something wrong. I am using V5 R15.
Column1 is "Width"
Column2 is "34in [length]"
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BPRASAD
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| 22 Feb 2006 09:43 AM |
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Try using the following. Create an excel Spreadsheet with only two columns, a couple of rows in the following way:
Column1 is "Width" -- No Quote
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Column2 is "34in" -- No Quote
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Go To Formulae icon and Click on "IMPORT" Button. Follow the prompts.
This would fetch the parameter "Width" and its length value 34in -- imported into your Part File from the Excel Spreadsheet selected. It works fine for me. I am using V5 R15.4. The problem may be due to the trailing part [length] specified after 34in. You don't need it. |
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Brian Prasad
COE-DPC/KBE Chairperson |
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COE-FORUM-USER
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| 22 Feb 2006 11:14 AM |
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| Thanks, I was able to get the parameters to work just by placing the units next to the number in the second column. I thought it needed the parameter type defined but it worked without it. |
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