Being Inventive

Tag clouds: are they useful?

We here at Autodesk think they are. Sometimes a picture says more than a thousand words. And that is exactly what tag clouds are all about.

As you might or might not know Autodesk recently added tagging capability to its newsgroup posts. Everyone can add personal tags or (preferably) reuse existing tags.It allows you to highlight which topics are important to you and it allows us to easily spot the more popular ones. Here are the tag results that I recently collected from the Inventor newsgroup:

 

By removing the obvious tags (Help, Error, Problem, Drawing, Assembly, Part, File), we can easily get a more refined view of what is going on on the Inventor newsgroup.

 

Outside the obvious big 3 (Part, Assembly and Drawing), I think there is a need for information or trouble shooting in areas such as Sketching, Content Center, FEA, Vault, iLogic, Frame Generator, Excel, iPart and BOM. Especially the presence of Sketching in this list surprised me.

Here is the same tagging technique used on the categories of this Inventor blog.

 

By comparing the two clouds,  we can make sure that the blog posts we create are relevant by matching them to the subject matter interest as formulated on the newsgroup.

I must admit that we haven't created any blog posts on Sketching yet (assuming that it was an easy to understand module of Inventor without too many problems). Maybe we need to revisit this approach and offer more sketch related articles. 

Let us know what you think of this conclusion.

Bob

Inventor Studio – Record Animation Time

You want to produce a video of your animation.

In the Inventor Studio environment, Render tab, Animate, you click on Video Producer.

 

Then you click on Record Animation.

 

In the following Render Animation dialog, Output tab, Time Range, if you select the option Entire production, and you get a video with 1 frame.

 

If you try to set the Specified time range, the end cannot be greater than 30 seconds.

 

 

If this is your case, make sure you have created a Camera.

 

Then, click again on Video Producer and drag the camera to the timeline.

 

Select the camera in the timeline and edit it.

 

Set the End time to the value you want.

 

Of course it cannot be greater that the entire animation time.

 Ale

Cost of Structural Components

You want to calculate the cost of a Structural Shape component based on a standard cost per meter x length.

The solution is to apply the following procedure for each Structural Shape family you are going to use in Frame Generator.

• Copy the family in a Read/Write library.
• Open From Content Center and insert one member of the family with the option As Custom.

 

• Go to Parameters dialog.
• Create a new User Parameter: CostPerMeter and set its unit to Unitless. Set the value according to your requirement.
• Create another new User Parameter: Cost and set its unit to Unitless. Set the equation for Cost to “G_L / (1 m) * CostPerMeter”.
• Check the Export checkbox for the parameter Cost.
• Edit the parameter Cost Property Format for not displaying the Unit String.

 

• In the CC Editor, Replace Family Template selecting this file.

 

• In the Family Table, define a new column and map it to the custom property.

  

After that, every family member generated with Frame Generator will have the Cost property in the Custom tab in iProperties and it can be referenced by BOM table.

   

And you can easily edit the Parts List if you want to display the total cost of all the components with the same length.

 

The video below shows all the steps described above.

 
 

Ale

Inventor 2012 Expand dialogs

You want that the following six dialogs (Extrude, Revolve, Fillet, Chamfer, Face draft and Move face) expanded automatically and permanently instead to display as in the image below when you click on the corresponding command.

 

In order to do that:

• Close Inventor.
• Control panel > System > Advanced System Settings > Environment Variables.
• Implement the following System Variable.

Variable Name: INVENTOR_ROLL_DOWN_DIALOG

Variable Value: YES

 

Note that this will not prevent you from temporarily collapsing any of these dialogs, but on the next use of the dialog, the dialog will come up in expanded mode as long as the variable remains set.
 

Export Inventor part file as OBJ file

You want to export an Inventor part file as OBJ file for using it in a 3D digital image editing program, as Maya, Mudbox, etc.

In order to do this:

• Download and unzip this VBA_Macro to your local drive.
• Open the VBA editor.
• File > Import and insert the file Ipt_Obj.bas into your application project.
• Open the part file to export.
• Run the macro CreatOBJFile.

 

• Enter the value for the density of the mesh.

 

• Save the OBJ file in the desired location.

 

Note. The VBA is just for single body part file.

Base view scale in title block

You want to incorporate the view scale of the first view on the title block of each drawing sheet.

 

For doing this:

• Download and unzip this ILogic Rule to your local drive.
• Create an iLogic rule, copying the script from the file you have downloaded, and run it.
  • The rule creates a custom drawing property called "Scale x" for the scale of the first view on each sheet x  (i.e.: Scale 1 on Sheet:1)
• For each sheet of your drawing,
  • Edit the title block definition and add a text that includes the custom drawing property called "Scale x" for the scale of the first view on sheet x.
  • Save as the title block naming it, for instance:  “Title block Sheet x”
  • Replace the existing title block with the new one created.
• Add the rule to an Event Trigger (i.e.: Before Save Document).

 

• (Optionally) save the drawing as Template.

In the video below you can see the workflow for creating a Template with two sheets. 

 

**************

Update: For an alternative method see the post below

http://beinginventive.typepad.com/being-inventive/2013/03/adding-scale-to-title-block.html

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Propagate item number override from subassemblies to parent assembly

When you override the item number in the BOM of a subassembly, you expect to find that same item number back in the BOM of the parent assembly.

However this override does not propagate into the parent.

 

Example in the BOM of a first level sub

Result in the parent BOM

 

For solving the problem

• Download and unzip this VBA Macro to your local drive.
• Open the VBA editor.
• File > Import and insert the file SyncBomItemNumbersModule.bas into your application project.
• In the parent assembly, enable the Structured BOM and set the Properties to "All Levels".

 

• Run the macro called "Sub SyncBOMItemNumbers()" and get the result.

 
 

If this is a common workflow for you, you may find useful to place the macro as an icon in the ribbon as follow

• Go to Tools > Options > Customize.
• Locate the macro by name (in this case "SyncBOMItemNumbers") in the left pane.
• If you want the macro to show up in the Assembly Assemble ribbon, select Assembly|Assemble above the right pane.

 

• Hit the >> button and set the Text checkbox.

 

Meaning of Remote Force in Stress Analysis

The best way to explain how to use a remote force is by example. Figure 1  shows a simulation of the torque applied on a screw by a wrench. The wrench is represented with the green sketch lines in Figure1. We are not interested in the actual geometry of the wrench, we are just interested in the position of the remote force and its effect on the bolt, that is why we limit ourselves to a rough 2D representation of the wrench.

 

Figure 1: Remote force applied on a 2D model of a wrench

A remote force is typically NEVER applied at the pick location on the face. By its nature the remote force will always be disconnected (at a distance) of the face that is initially selected.

The default position of the remote force is 0,0,0 and the direction is perpendicular to the face that is selected. The reason why we picked 0,0,0 is arbitrary. The only reason I can think of is that we wanted to convey that a remote force is not the same thing as a regular force.

Let's continue with our example of torque which has following relationship to the force

 

                torque = remote force x distance

 

If we place a remote force of 5 Newton on a face of the bolt at a distance of 100 mm from the center of the bolt, we get a torque of 5 x 100 = 500 Nmm.

And if we then create a second similar remote force on the opposite face of the bolt (to simulate the working of a wrench), we can calculate the maximum stress on the faces of the bolt: 4.88 MPa.

 

Shaft calculation after adding grooves, keyways or chamfers

Shaft generator calculations are based on the shaft section as shown in the 2D preview window.
This might not always be obvious especially when you start adding certain extra features to the shaft.

In Figure 1 you can see that some features present on the left side of the 3D model are not represented in the 2D calculation preview in Figure 2.

 

Figure 1: 3D model of shaft

 

Figure 2: 2D model of shaft (used for calculation)

The explanation is that any feature that adds material to or removes material from the shaft like a chamfer, a fillet, a groove or a keyway, will not be used in the 2D shaft calculation.

To obtain more advanced calculation results, use the Stress Analysis module rather than the Shaft generator module.  

Use of 3GB switch with Inventor 2012 on 32 bit machine

Autodesk does not support or endorse the /3GB switch on 32 bit machines.

In many cases, this customization will cause Inventor graphics to be incorrectly displayed.

The new enhancements for marking menu, mini toolbar & select other “may” all consume more memory than their 2011 equivalents.

Instead, we recommend updating to a 64-bit version of Windows as reported as well in the Wiki Help under Autodesk Inventor 3 GB feature (Applies to 32-bit operating systems only)