Being Inventive

Welcome to the Inventor support blog!

 This is a blog maintained by the Inventor product support group at Autodesk.

We plan to cover a plethora of subjects that we come across in our daily work, starting with the most recent 2012 release of Inventor but we will not shy away from topics going three releases back.

We hope our experience will be also your gain and that the posts we will publish here will make your life with Inventor even more pleasurable.

And remember: be inventive with Inventor.

Bob

Adding Multiple Components in iAssembly Table in batch mode

You want to convert your assembly in an iAssembly.

You have many components that need to be configured for Include/Exclude.

If you don’t want adding them one by one in iAssembly table, you can try the steps below.

• Convert the assembly to iAssembly and click OK for closing the iAssembly table

• In the Manage tab, Author, switch to “Edit Member Scope”

• Select multiple components in the assembly browser, right click and select “Exclude”

The columns corresponding to the selected components will be added into iAssembly table.

Then, you can switch back to “Edit Factory Scope” and Edit the iAssembly table for making the adjustments.

Ale

Adding Scale to Title Block

Sometime ago we have published the post below that allows to add the scale value from the first view on the sheet and put it in the title block, using an iLogic rule.

http://beinginventive.typepad.com/being-inventive/2011/06/base-view-scale-in-title-block.html

We have appreciated all the positive feedbacks received about the post, but also the concerns you have sent us about some limitations of the proposed solution.

The main one is that you have to create one different title block for each sheet, and, especially if you need to delete and add sheets to your drawings or templates, this is not practical.

So, the new solution proposed below doesn’t require the creation of a new iproperty to be added to a new title block for each sheet.

This is a simpler method that uses Prompted Entry text in the title block instead of an iProperty. 

In order to apply the new solution, do the following.

• Edit your title block definition and add a Text item with the type Prompted Entry

• This text should contain <Scale>

After you add this, Inventor will prompt you for a Scale value whenever you add the title block to a sheet.

The same happens when you add a new sheet with the title block to the drawing or when you start a new drawing using a template where you have applied this solution.

• When it prompts you, just leave the value blank

• Then add this Rule to the drawing

• Add the rule to the trigger “Before Save Document”

After that, on every sheet in the drawing, you will get the scale value from the first view on that sheet in the title block when you save the file.

Special thanks to Mike Deck for suggesting this new solution.

Ale

Associate by default materials to solid hatch in section views

You have an assembly view in your drawing.

You want to create the section view of it and apply automatically a solid hatch to the components with specific materials.

In order to do that, please follow the steps below.

• Download SOLID.zip and extract the PAT file in a location on your machine

• In the drawing file, open the Style Editor

• Select the Hatch style for the active standard

• In the right side of the dialog, open the drop-down menu for the Pattern and click on Other…

• In the following Select Hatch Pattern dialog click on Load

• In the following Load Hatch Patterns dialog, browse to the PAT file you have downloaded and load it

• After that, the solid hatch should be in the list of the loaded pattern and selected

• Click OK for closing the dialog

• Now the Solid hatch should be the default Pattern for the active hatch style

• Set the default Pattern back to the usual one (i.e.: ANSI 31) and save the Style edits

• In the Style Editor, select the active standard and in the right side of the dialog, select the Material Hatch Pattern Defaults tab

• Add the name of the materials you want to associate to the solid hatch
  • Alternatively, in the Import Materials section, you can import the materials from a part file, clicking on From Files… and selecting the part that contains the materials in the part document or from the active Material Style Library, clicking on From Style Library  

• Change their hatch Pattern from the drop-down menu and set them to Solid

• Save the edits in the Style Editor

• Then, create the section view of the assembly and get the solid hatch for the components with the specified materials

 

Final notes.

You can save these settings in the Style Library if you want to get the solid hatch associated to the specific materials by default in all the new drawings you create.

In case, after doing that you get the Style Conflict message opening a drawing template, read this post for solving the problem.

Of course, these settings apply also if you create the section view of a part with one of the materials specified.

 Ale

Add Density Property to Parts List & BOM

You want to add the component physical property of Density to the BOM and Parts List for your assemblies.

In order to do that, you need to follow the steps below.

Define the Custom Property in the components of the assembly as in the image below.

The name of the property is not important, but cannot be “Density” or “DENSITY”.

What matters is the value that must be “=<Density>” and you can add the units if you want to display them as well.

You can save this property in your part template file, so that you have it in every new part you create.

Then, in the assembly, add the Custom property column to the BOM.

Even in this case, you can save this setting in your assembly template, so that the column will be available and display by default in the BOM of each assembly you create.

Finally, in the drawing, edit the Parts List style adding the custom column.

Edit the format of the column and rename the column heading.

You can save these settings in the Style Library if you want the column available by default in the Parts List of all the new drawings you create.

Ale

Lines in the view are stretched after conversion to AutoCAD DWG

In Inventor 2013, you have a drawing where the views display, for instance, some nuts.

You export your drawing as AutoCAD DWG, but opening the resulting file in AutoCAD, some lines display incorrectly.

Our Development is working for fixing the problem in one of the next updates.

 

In the meantime, I hope you can find useful the following workaround.

• In Inventor, open any drawing

• Export to DWG

• In the Export to DWG dialog, click on Options

• In the following dialog, click Next

• In the next dialog (Export Destination) click on Save Configuration…

• Name the ini file and save it in a location on your machine

• Click Cancel for exit the exporting process

• Edit the ini file with Notepad

• Find the line "REPLACE SPLINE=No", change the No with Yes and save the file

Once you have created and edited as explained above the ini file, you can use it for exporting the “problematic” Inventor drawings as AutoCAD DWG.

For doing that, you need to click on Options in the Export to DWG dialog and load the configuration file you have modified in the following dialog.

Then, just click Finish and save the file.

 

Caveat. This change on exporting setting will impact all spline objects, replacing spline with polylines.

So, if you want to go back to the default behavior exporting “non-problematic” Inventor drawings, in the Options you can set the Default DWG Configuration or your usual configuration file.

Ale

Environment variable "InvCM_ForceConvertToGeneric" to convert legacy colors to generic type in Inventor 2013

Inventor 2013 is using the Autodesk Material Library to provide a smooth appearance experience across the Autodesk Products.

However, you may see differences when migrating your files from older Inventor Release to the latest one. Bob wrote this Blog article  about the color topic in Inventor 2013.

In fact, the Autodesk Material Library was already available in Inventor 2012. You could access it in the Styles and Standard Editor, Field Realistic Appearance.
In most of the standard colors, the Realistic Appearance option was checked, but you had to enable the Realistic Appearance Mode to see it in the Graphic window.

 

Realistic apperance option and realistic visual style in Inventor 2012 

 

When migrating to Inventor 2013, you will see the realistic appearance. It might be looking differently than what you were seeing in 2012 classic shaded mode.
If you have standard colors in your 2012 document, they will get converted to our new 2013 standard colors (find the conversion table in Bob’s Article). So it will get another name and might look differently.

For example standard “Glass (Limo Tint)” becomes “Light Gray Reflective” in 2013.

The 2012 Colors style settings are no longer valid and we will use the realistic settings. You will see a much darker color shade, which matches what you would have seen in realistic mode in 2012.

Plus “Light Gray Reflective” will belong to the appearance category Glass/Glazing which has specific controls as you can see in the screenshot. Other categories will have other type of controls.

Glass Limo Tint in 2012 becoming Light Gray reflective in 2013

 

A new environment variable was provided in 2013 SP1.1 "InvCM_ForceConvertToGeneric" (value set to 1) that will maintain appearance names, ignore any realistic settings and convert all appearances to a generic type.

So if you migrate “Glass (Limo Tint)” with the variable in 2013, you will get a new appearance called “Glass (Limo Tint)” in the generic category and using the 2012 Color style settings.

 

 Environment Variable and Migration result of Glass Limo Tint with the variable

 

Usually the appearances in 2013 are darker, transparency can be different with the Glazing settings.
Use this variable if you want to minimize the difference between Shaded View in 2012 and Realistic Appearance in 2013. The appearances will be converted to generic type, which exposes all controls, and gives you more possibility to fine tune your visual results.

You will have to implement this variable on all your computers. Migrate once your custom library with the variable, and let the variable in case you get documents with local styles.

This variable doesn’t affect the materials.

Pierre.

Reference part in assembly showing through other components in drawing views

You have created an assembly defining one part as Reference.

Then, creating a drawing with the assembly views you notice that the reference part is not hidden by the other components and vice versa.

So, if you want that the non-reference body hides the reference one and vice versa, you need to do the following.

• Edit the view
• In the Model State tab, set the Hidden Line Calculation for the Reference Data to “All Bodies”

After that, the views display as expected.

Ale

Empty Part Number for Content Center Library components

When you insert a component from a Content Center Library family either with the command Place from Content Center or with Frame Generator you want that the Part Number field is empty.

In order to do that,

• Copy the family in a Read/Write library

• Select the family you have copied, right-click, Family Table.

• In the Family Table, select the Part Number column, right-click, Column Properties.

• In the Column Property dialog set the Expression Column field to “=”

• Publish the changes.

After that, inserting a member of that family either with the command Place from Content Center or with Frame Generator you will get an empty Part Number field.  

Note. If you have modified a Structural Shape family as described above and you generate the members with Frame Generator, you need to select the box "Get Frame Member's Part Number from Content Center" in the Insert dialog for getting the empty Part Number for the frames.

By the way, the box is checked by default.

For more information about this option you can read this post.

Ale

Update 1 for Inventor 2013 SP1.1 has been released

Update 1 for Inventor 2013 Sp1.1 has been released:

http://usa.autodesk.com/getdoc/id=DL20857064

Please, read the Readme file for the description of the issues addressed and the installation instructions.

Assembly Section Views Afraid of Commitment in 2013

After seeing enough users struggling with an issue in 2013 and it being deemed as designed for 2013, I thought it necessary to point some commitment issues out that section views are having in this release. This is largely due to the mini toolbar associated with section views and the continue button without an “OK” button in sight.

You start your ½, ¼ or ¾ section (we’ll use half section in this example due to its one work plane needed) then see the continue button on the mini toolbar after picking the work plane and pick it. But the next click you make takes you into a full view of your part again with no indication that you haven’t committed to the section view but, rather, have ended it in favor of your next command:

Ugh!

This is due to the fact that, by not right-clicking and selecting “OK” or clicking the enter key, after clicking continue Inventor 2013 has decided you did not want the section after all.

 

So as a helpful hint: before moving on (and out) of the section view and in ending it inadvertently, RMB and choose OK to force it into commitment.

There are tentative changes to the 2014 release to make this much more intuitive and those of you that are Beta testing have seen what I mean already.  I hope that helps keep the frustration level down a bit.

 

-Daren