View / scale controlled value

[Jersdunz]

I want to be able to use a paramater in the iproperties tool box to control the view scale of all my base views when creating cut files. All parts in a cut file must be of the same scale. Scaling is an issue when lasering dozens or hundereds of parts. I'd like to be able to open the iproperties tool box and change a value and have all associated views change scale accordingly.

I use the =<sheet metal rule> in description to control the designated material call out in each parts description but my scales are all manually entered and there fore open for error. Is this possible? Please see included image

[blair]

We either export the file directly from the IPT file for all our profile cutting. Even placing the part in a IDW and doing a Save-As to a DWG and then opening the DWG and selecting the geometry and exporting to a DXF still gives the correct size for cutting (required for some stupid Spline-Lines).

99% of our NC tool-path files are from a straight export to IGS and then imported into our NC tool-path software.

[Jersdunz]

We try to use only flat patterned sheet metal parts in our cut files. Then we'll save copy as to autocad dwg and clean up the ose rediculous splines. (the splines are less anoying to me than the blown up text / title blocks) I couldn't even begin to imagine how tedious it would be, to use iges files.

Right now I have the description of a part referencing its sheet metal rule parameter. So if in the model a part gets changed from say 10 ga to 1/2"  the label in the idw cut file us automaticly updated. But each base view placed in the idw file had to be specified a certain scale.

Then the project grows and you need to create more room in the cut file for additional parts by scaling the views and that opens the draftsman ( myself ) up for key entry error. Its not fun when 20 parts get cut from 3/4 plate that should have been 12 ga as an example.

Still seeking an answer for this desired function.

Use a paramater from the idw files iproperties to dictate scale to all included base views.

I know there has to be a way to do it, I just can't find it.

[blair]

Our ERP system references the pattern only and the order calls for the material and thickness.We could have 20 different part numbers with a BOM in our ERP system for each part number. Since the job is created in the ERP system, it lists the materal to be used and the pattern number required and any drawings.

We could use the same pattern for all the parts. No need for the operated to look at the drawing for that information.

We IGES out the shape directly from the IPT file within Inventor (Export) and our tool pathing software directly reads the IGES. No problems at all.

[jtylerbc]

This isn't exactly what you're asking for, but I've got a macro I picked up somewhere that will change all the views on a sheet to some entered value (which it prompts you for).

Example:  You want all views at 1:2 scale.  Run the macro, type ".5" into the input box, click OK.  All views on the current sheet change to 1:2 scale.

Does your solution really need to be parameter-based, or would something like that work for you?

[Jersdunz]

that sounds like it would work fine .. might not be what I was going for but it accomplishes the same thing..

Autodesk should certainly look into this function for the next release though for sure.

[jtylerbc]

Attached are the VBA files for the macro and the dialog box form.  Import them into your VBA editor, then you should be able to run it.

Hopefully this will help you out.

[Jersdunz]

thanks i'll keep you updated.

[jeffrey.sun]

Hello Jersdunz,

The view scale can be automatically updated by iLogic Rule.

The workflow is

1. Open the drawing document.

2. Add a numeric parameter, name it myScale. Select the unit type as unitless.

3. Add an iLogic Rule. Name it ChangeViewScale.

4. In the rule, add the code like (The actual view names depend on the actual name you set)

ActiveSheet.View("VIEW1").Scale=myScale
ActiveSheet.View("VIEW3").Scale=myScale

5. Click OK to save the rule.

6. Open the parameters dialog, change the value of myScale to a different one.

Result: The scale of the views on the sheet will be updated.

The steps above is an example how to use the iLogic to implement automation.  Of course it supports more complicated operations.

[Jersdunz]

thanks Jeff, Would there be a way to word

the ("view1") text in the rule to include all views on a sheet or in an entire drawing file?

[jeffrey.sun]

Hello Jersdunz,

Add the code below to the iLogic rule. It can traverse all the views in the active sheet.

Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

Dim oView As DrawingView
For Each oView In oDrawDoc.ActiveSheet.DrawingViews
If Not oView.ScaleFromBase Then
oView.[Scale] = myScale
End If
Next