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Help - Parametric control


paulhea

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Hi All,

 

Can anybody help with the following. I have thousands of these tiles to produce in different sizes. The only variables will be the length, currently 660mm, the width, currently 220mm and the end angles, currently 55.97 degrees.

I am trying to control parametrically these 3 dimensions however I am getting update errors when I re-populate these fields.

 

 

Thanks

 

P

Part1.ipt

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Stitch.PNG

I am having trouble understanding all of the Work Planes and Splits?

Can't you simply Stitch surfaces and then cap the ends with Patch(es) and Sculpt or Stitch to get your solid body?

 

Can't you re-use Sketch1 for the Extrusion?

 

Edit:

I dug a little deeper and see that your 3D sketch is not fully defined.

You will need to Include Geometry from your 2D sketch into your 3D sketch to fully define the sketch.

 

Defined Sketches.jpg

 

Note the sketch color for your 2D sketch vs the color for your 3D sketch.

You will never get predictable behavior without fully defined sketches.

 

Edit your 3D Sketch.

Drag the green lines a bit away from the intended connection points

Add Coincident constraints between the intended connection points between the 2D sketch and the 3D sketch.

Do this on every corner till all lines turn dark color (full defined).

Coincident Constraints.PNG

Edited by JD Mather
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  • 2 weeks later...

Did you ever resolve this part? I applied JD Mather's changes and uploaded the part in case you need it. Also, you mentioned you have a bunch of these to make. Are you aware that you can use Excel spreadsheets to control the parameters of models? That may make such a mass project significantly easier. I'd be happy to help you figure it out if you think it would be beneficial.

Part1.ipt

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Did you ever resolve this part? I applied JD Mather's changes and uploaded the part in case you need it. Also, you mentioned you have a bunch of these to make. Are you aware that you can use Excel spreadsheets to control the parameters of models? That may make such a mass project significantly easier. I'd be happy to help you figure it out if you think it would be beneficial.

 

 

Many thanks for your response and attachment. Much appreciated.

Yes I did know you can use excel spreadsheets but haven't had much success

in doing so and at the moment I inly have access to open office version of it.

Can it be done with this?

 

Kind Regards

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Definitely. All Inventor needs is a basic .xls or .xlsx file. Most of the work involved is done by Inventor and not Excel, so Basic is more than enough.

 

Make a new Excel workbook and put your parameter names in column A and values in column B. In Inventor, open the Parameters window and click "link" at the bottom left. Navigate to the workbook and click "open". Inventor will automatically import your parameter names and values into custom parameters that you can use in your model. When you're sketching and extruding, you can type in your parameter names where you want those values (case-sensitive). Then, any changes in that Excel file will automatically cause the Inventor part to change also. I attached screenshots of my process. Let me know if you have any trouble with it.

1.PNG

2.jpg

3.jpg

4.jpg

5.jpg

6.jpg

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Inventor ONLY uses MS Excel.

From system requirements for Inventor 2018

•Full local install of Microsoft® Excel 2010, 2013 or 2016 for iFeatures, iParts, iAssemblies, thread related commands, clearance/threaded hole creation, Global BOM, Parts Lists, Revision Tables, spreadsheet-driven designs and Studio animation of Positional Representations. Excel Starter®, Online Office 365® and OpenOffice® are not supported.
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When you're navigating to the spreadsheet, there's an option at the bottom of the window to either link the Excel file externally or embed it. In this case, you want the "link" option. Right click and "delete folder" on the embedded spreadsheet in Parameters, and link again, choosing "link" instead of "embed" this time.

Capture.PNG

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When you're navigating to the spreadsheet, there's an option at the bottom of the window to either link the Excel file externally or embed it. In this case, you want the "link" option. Right click and "delete folder" on the embedded spreadsheet in Parameters, and link again, choosing "link" instead of "embed" this time.

 

 

Thanks, That was the method I originally used but still get the same error

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No, it's always been that way with Inventor, you MUST HAVE MS Excel, no other will work, never has.

 

System requirements for Autodesk Inventor 2017 products

•Full local install of Microsoft® Excel 2010, 2013 or 2016 for iFeatures, iParts, iAssemblies, thread related commands, clearance/threaded hole creation, Global BOM, Parts Lists, Revision Tables, spreadsheet-driven designs and Studio animation of Positional Representations. Excel Starter®, Online Office 365® and OpenOffice® are not supported.
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