Sheetmetal styles dialogue from iLogic

[Anonymous]

I am creating part templates for some standard sheetmetal sections which will in turn be used by some semi-skilled users to set the material and gauge from the sheetmetal styles and then set various part parameters (say width height and length. 

I'd like to open the inventor sheetmetal styles to allow the user to select a predefined style and then once the style is set, defining the material and gauge they will set the part parameters (say Length, Width and Height). See attached JPg for form example.

Thanks in advance for any help.

Regards

Richard

[Anonymous]

Okay, from what i understand, you define the sheet metal style from your template. 

Or else I guess that you have to educate the less educated users how to work with the Style and Standard Editor; if you want them to handle options regarding sheet, thickness, bends and corner cuts. 

As a new user it looked intimidating, but it took less than a day to learn it... and I had only myself to help me.

The manufactored details came out exactly how I wanted them to.

Have a nice day! / Ola

[doug.johnston · Accepted solution]

I think I have something similar to what you are looking for.

It is a form with custom user parameters that is pulling most of the information from an Excel spreadsheet that was I created.

I do a lot of sheet metal parts, so I created the spreadsheet to match my workplace naming convention "SHEET METAL INFORMATION" section.  All the information is generated from selecting the "Material Number" which gives the "Material Description" / "Material" / "Material Gauge" / "Material Thickness".  The weights are generated from the "Width" and "Length" parameters which ties to a "lbs/sqin" column on the spreadsheet.

Is this close to what you are looking for ??

[Anonymous]

Hi Ola,

Thanks for your reply. What I need to do is restrict the no of options that the user has so they can only use the options in the sheetmetal style of the template. I think the easiest way to do this is to do it through iLogic driven forms.

Thanks for your help.

Cheers

Richard

[Anonymous]

Hi Doug,

This is very nice and pretty well does most of the stuff I want. Is this done using iLogic or is it VB. Nice solution either way. Is all the material info loaded from your Inventor Sheetmetal style?

Thanks and Regards

Richard

[Anonymous]

Hi Doug,

I reckon this does what I want. I'd love some code to go with it. Just restarted doing VB after a long break and It's taking a while to get my head around the new object models.. Thanks for your help.

Regards

Richard

[doug.johnston]

Good morning Richard,

Sorry for not responding sooner, it was a very busy week.

Here is my code where I am reading the excel spreadsheet to get the appropriate parameters.

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'' Rule is reading and importing iproperties from SHEET METAL INFORMATION Excel spreadsheet

''define Excel spreadhseet location, "MATERIAL_NUMBER" multi-value list and cell range
MultiValue.List("MATERIAL_NUMBER") = GoExcel.CellValues("C:\00-GUSPRO_Vault\02-CAD FILES\WATERJET\SHEET METAL INFORMATION.xlsx", "Sheet 1", "A2", "A70")

''define custom iproperties from spreadsheet columns based on "MATERIAL_NUMBER" selection
i = GoExcel.FindRow("C:\00-GUSPRO_Vault\02-CAD FILES\WATERJET\SHEET METAL INFORMATION.xlsx", "Sheet 1", "MATERIAL_NUMBER", "=", MATERIAL_NUMBER)
MATERIAL_GAUGE = GoExcel.CurrentRowValue("MATERIAL_GAUGE")
MATERIAL = GoExcel.CurrentRowValue("MATERIAL")
MATERIAL_DESCRIPTION = GoExcel.CurrentRowValue("MATERIAL_DESCRIPTION")
MATERIAL_WEIGHT = GoExcel.CurrentRowValue("MATERIAL_WEIGHT")
TAB_WIDTH = GoExcel.CurrentRowValue("TAB_WIDTH")
MATERIAL_THICKNESS = GoExcel.CurrentRowValue("MATERIAL_THICKNESS")
WEIGHT_SQFT = GoExcel.CurrentRowValue("WEIGHT_SQFT")
WEIGHT_SQIN = GoExcel.CurrentRowValue("WEIGHT_SQIN")

''create custom iproperties in sheet metal template
iProperties.Value("Custom", "MATERIAL_NUMBER") = MATERIAL_NUMBER
iProperties.Value("Custom", "MATERIAL_DESCRIPTION") = MATERIAL_DESCRIPTION
iProperties.Value("Custom", "MATERIAL_GAUGE") = MATERIAL_GAUGE
iProperties.Value("Custom", "MATERIAL") = MATERIAL
iProperties.Value("Custom", "MATERIAL_WEIGHT") = MATERIAL_WEIGHT
iProperties.Value("Custom", "TAB_WIDTH") = TAB_WIDTH
iProperties.Value("Custom", "MATERIAL_THICKNESS") = MATERIAL_THICKNESS
iProperties.Value("Custom", "WEIGHT_SQFT") = WEIGHT_SQFT
iProperties.Value("Custom", "WEIGHT_SQIN") = WEIGHT_SQIN

iLogicVb.UpdateWhenDone = True

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Here is the Excel spreadsheet (see attachment)  ... 

I am using all ilogic in the rule and no VBA code.

Of course, you will have to create your own spreadsheet to match the parameters you want, but it is a very simple program to modify.

After creating the custom iproperties, you can create the form to grab whatever iproperties you want to include.  My form only allows the "MATERIAL_NUMBER" to be selected by the use and all the other values are "greyed out" to show the information only.

I have another couple of rules to calculate "LENGTH, WIDTH and THICKNESS" and "WEIGHT" based on the "WEIGHT SQ_IN" values.+

EDIT - I only use one standard sheetmetal style, so I don't need to change the styles to match my individual materials.

If you would like any more information or assistance, let me know.

Thanks,

Doug J.

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[Anonymous]

Thanks Doug,

This should help to get me out of a hole.

Regards

Richard

[doug.johnston]

No problem.

If you need any more help, let me know and I can help you change the code / spreadsheet to suit your requirements.

[Anonymous]

Thanks Doug. I should be pretty right now. I'll let you know.

Regards

Richard

[beth.maddux]

I Have a quick question about this. I am trying to go a step further and have it when I make the selection from the drop down that then changes my sheet metal defaults. Is that possible? Those sheet metal defaults for us contain the K factors and control our part thickness. I was really hoping to have that as an option where my users can just us the form to do everything.