Being Inventive

Adding a little class to threaded iParts

You’ve made an iPart with a hole and thread feature that can change sizes between ANSI Unified, Metric, etc. and added the thread information to the table so the part will update and the thread specification changes based on the thread. But when you change to from one member to another with a different standard, you get the following warning:

You’ve got the right thread designation and type, the tap drill size is correct or at least close so you shouldn’t be seeing this warning, right? Yes, with a catch. After the switch you’ll also see the thread warning in the browser:

So you check on the thread specification and change it to the correct designation. Next you go to edit the table to double check and are faced with the following warning:

If you choose “Yes” you’ll get the warning when changing back to a different thread type and it may even change all your thread types in the table. So what can you do to get it to recognize the thread specification? Add the thread class to the table. For instance, if it’s an ANSI English thread, you can change the class to “2B” and use “6H” for metric holes. If you’ve got a number of rows, you can edit in Excel and use the drag copy to set all the values to the appropriate rows.

Now, once you verify and click “OK”, you’ll notice no more warnings as the thread specification switches as you change members.

I hope that’s helpful. Happy New Year!

-Daren

iPart Origin work features visibility

You have created an ipart and purposely left some origin work plane and axis displayed for alignment purposes upon insertion, but, when you insert an ipart member into a new assembly the work feature do not display and the option to turn the  visibility on is not available.

This should not be a problem for positioning the ipart member in the assembly, because even if the Origin work features are not visible you are still able to select them in the browser for defining constraints.

By the way, if you want to display the Origin work features inserting the ipart member in the assembly you have three options.

1. Create an imate for each Origin work feature you want to display, selecting it.

Then, add the imates to the ipart table.

After that, inserting the ipart member in an assembly, the work features will be visible.

2. Create user work features which are coincident with the origin work features.

Then go to the "Work Features" tab on the iPart Author dialog, add a column to your iPart table for the new work features, and set the table values to "Include".

3. Define, at least one column in the iPart, as Custom Parameter Column.

In this way, the option to turn the ipart member origin work features visibility on will be available in the assembly environment.

Ale

Excel Starter and Inventor

In the Inventor 2012 System Requirements, we can read this concerning Excel:

…

Microsoft® Excel 2003 through 2010 for iFeatures, iParts, iAssemblies, thread customization, and spreadsheet-driven designs

…

There is however one exception to this system requirements paragraph that is not mentioned explicitly and we just found out about this exception via one of our beta testers: the free Microsoft product called "Microsoft Excel Starter" cannot be used with Inventor as a replacement for the full Microsoft Excel (which is of course not free).

The explanation is relatively simple.

Microsoft Excel Starter comes with the OEM version of  Microsoft Office 2010 (named Office Starter 2010) and gets installed as a "virtual application".

Because of this, the app does not register itself in the Windows registry.

And this means that Inventor cannot find Microsoft Excel Starter via the Windows registry and thus iParts/iAssemblies, iFeatures and threads will not function properly with Inventor.
You will have to upgrade to the full Excel product to make things work.

Conclusion: there is no free iLunch.

 

Inventor File Reserve 2012

You want to convert legacy Shared or Semi-Isolated projects to Vault or Single User projects, but some of the files in the project are reserved / read-only.

The attached tool allows you, between other functionalities, to un-reserve in one go all the files of the project.

For using the tool, download FileReserveR2012 and extract the files on your machine.

Read very carefully the readme file before using the tool.

Rename the file FileReserveR2012.___ to FileReserveR2012.exe.

The tool works with all older Inventor versions (from R6 – R2012).

Below you can find more details about some of the functionalities provided by the tool described in the readme file as well.

• Remove or Apply reservation flags from Inventor files.

UserXY owns the files.

   

Context menu or File Menu will provide Check In / Out functionality.

• Remove or Apply reservations from different users.

All selected files can be processed in one go.

• Search for all files from project (*.ipt, *.ipn, *.idv, *.iam, *.idw / *.dwg)

• Indicate files which have been created with Student version.

True = Educational file

False = non educational file

Not available = File Reserve used with Inventor Release < 2010

The tool, of course, doesn’t change the Educational condition of the file.

Change the Ground Plane orientation in your template

When you start a new assembly or part file, selecting your template and enable the Ground Plane visibility, this is oriented parallel to the XZ work plane.

If you want to change the default orientation and set it parallel, for instance, to the XY work plane and saving the new setting in your template, you can do the following.

• In the top right corner of the graphic window, click on View Face.

• In the browser select the XY work plane under the Origin folder.

• Right-click on the ViewCube > Set Current View as > Top.

• The Ground Plane will be oriented parallel to the XY work plane.

• Save the file as Template and replace your template with the modified file.

Next time you start a new file selecting this template and enable the Ground Plane visibility, the orientation will be parallel to the XY work plane.

Ale

Radian angular dimensions in drawings

You want to apply the angular dimensions in radian in your drawings.

You can set this in the model sketch, but not in the drawing dimension style.

Retrieving the dimensions from the model sketch in the drawing doesn’t help either.

The dimensions will be applied according to the active drawing style format.

By the way, if you want add the Radian values to the existing dimensions as alternate unit, you can do the following.

• Download and unzip this VBA Macro to your local drive.
• Menu Tools > Options > VBA editor.
• Expand the ApplicationProject so that you see the Modules.
• Insert a new module.
• Copy and paste the macro text in the module.
• Return to Inventor.
• Go to Tools > Options > Customize > Ribbon tab.
• Locate the macros by name in the left pane.

• If you want the macros to show up in the Drawing Annotate ribbon, select Drawing | Annotate above the right pane.
• Hit the >> button and set the Text checkbox.

Once you have completed the procedure above, you can open a drawing where you have already applied the angular dimensions according to the active style or apply them.

Then, in the Annotate ribbon, click on the command AddRadiansdToAngularDimensions and get the Radian values as alternate unit.

If you want to remove the Radian values, click on the command ResetAngularDimensions.

Ale

How to mind your P’s and q’s ?

Sometimes questions pops up around Inventor's calculation of beam deflections in the Stress Analysis environment.

Everyone knows the theoretical formulas from our school days. But not everyone knows how to correlate these schoolbook formulas to Inventor's way of defining loads and boundary conditions.

Let's take an example of a single point load in the middle of an I-beam.

 

Fig 1: Schoolbook formula for a suspended beam with a central point force

The concrete data that we want to use in these formulas are:

• P= 32000 N
• L = 9000 mm
• E = 220 GPa = 220000 N/mm^2
• I = Ix = 182630000 mm^4

The Ix value can be found in the region properties of the I-beam cross-section:

Fig 3: Identifying the moment of inertia values of the beam

With these numbers the theoretical deflection in the middle of the beam is:

d = 32000 x (9000)^3 / 48 / 220000/ 182630000 = 12 mm

Let's now verify if Inventor's Stress Analysis gives us an identical result.

Without too much thinking, the majority of our users will translate the schoolbook sketch as follows:

• A force of 32000 N applied to the top face
• A fixed constraint on two edges at both ends of the beam

Fig 4: Initial setup of the load and boundary conditions

If you run the simulation and look at the displacement results in the Y direction, you will see that the maximum displacement value obtained is 4.37 mm

Fig 5: Y displacement results with initial setup

Why do we have this large discrepancy between the calculated (4.37) and the theoretical value (12.0)?

Well the reason is that we made two fundamental mistakes in the way we applied the load and the boundary conditions.

• First the force P we defined is not really a single point force but is a force applied to the entire face and becomes more of a distributed q force (hence the title of the articleJ).
  

  So instead of using a point load P=3200 N, we actually performed the calculation with a distributed load q = 3200 N/ 2.7 m^2 = 11851 N/m^2 (with 2.7 m^2 being to top surface area of the beam).
  This can easily be verified by using a pressure force of 11851 N/m^2. You will get the exact same result as when using the P= 3200 N force on the top face.
  It is too bad that Inventor does not change the load glyph to convey more clearly to users what is going on.

• Second mistake is that we clamped down both endpoints of the beam by adding fixed constraints.
  If you look carefully in the schoolbook example, one endpoint of the beam can freely float in the longitudinal direction.

The first problem can be remedied by applying the force to a small circular split face in the middle of the beam's top face (note that you cannot apply a force to a sketch point or a work point):

Fig 6: Applying the force to a tiny centrally located circular split face (marked in brown)

The second problem can be fixed by defining a fixed constraint on one end and a frictionless constraint on the other end (but this again would require you to create a small split face near the beam's end)

A more convenient solution when the beam is suspended in horizontal fashion, is to simply allow the Z-direction of the fix constraint to float by unchecking the z checkbox in the advanced options

Fig 7: Allowing a fixed constraint to float in the Z direction (= longitudinal direction of the beam)

If we then repeat the calculation, we get a deflection of 12.46 mm which is much closer to the theoretical result of 12 mm.

This value can be improved upon by refining the mesh and by allowing more mesh refinement steps in the convergence settings.

Fig 8: Y displacement of 12.46 mm after modifying loads and constraints

Missing a dialog box?

This issue comes up so often and just did again today, that I thought I’d share a trick. Suddenly the hole or other dialog is no longer visible when you summon its command. The dialog(s) may be off-screen as a result of working with dual monitors, placing the dialog(s) on a second monitor and having switched back to a single monitor. Even if this isn’t the case, they could have been inadvertently dragged or placed outside the viewing area. The trick is the following:

• Invoke the hole command (or any command experiencing this issue)
• Hold the alt key and click the spacebar, then release both
• Without doing anything else, press the “M” on your keyboard (move)
• Without doing anything else click one of the arrow keys on your keyboard
• Now move the mouse around without clicking any mouse buttons because the dialog box will be attached to your cursor and left click when you’ve got in a place where it’s visible.

This technique can be used on any Microsoft-style dialog box and in any application for that matter.

Daren

Frame member Family information in BOM

You want to include the “Family” information of a frame member in the Bill of material of your Assembly.

In order to include this information in the BOM and, in case, in the Parts List, you can do the following.

• In the assembly BOM, add a new Custom iProperty column.

• Name the new iProperty column, for instance, Family Name, and set the Data Type to Text.

• Select the first cell of the Family Name column and click on Create Expression.

• In the following Property Expression dialog write the expression “=<Family>” and then click OK.

• Select the lower-right corner of the first cell and drag it down to the last column cell, applying the same expression to all the other cells.

In the Frame member rows, the Family name will appear in the cells.

 

Alternatively, you can get the same result doing the following.

• Copy the Family of frames in a custom library in the Content Center Editor.
• Edit the Family table and add a column with the properties as in the image below.

In this way, you will get the custom property for each Frame member you insert from the Content Center or Frame Generator.

The advantage if this alternative method is that you can create an assembly template that contains in the BOM the custom iProperty column "Family Name".

For doing that, you just need to start a new assembly, go to the Bill of Material, add the new Custom iProperty column and save the file as Template

Starting an assembly with this template and inserting the frames from a Family modified with the alternative method, the Family Name column cells corresponding to the frame members rows will display the family name automatically.

The disadvantage of the alternative method is that you need to copy in a custom library and modify each Family of frames you are going to use.

 

Once you get the Family Name in the assembly BOM using one of the methods above, you can easily add the column in the assembly Parts List in the drawings.

Ale

Calculating developed length for sheet metal bends larger than 90 deg

This question comes up regularly as users want to double check the developed length of their sheet metal parts.
The Inventor wiki help shows all kind of nice pictures and formulas for the developed length but if you look more closely you will notice that all the images provided in the wiki are for situations where the bend angle is smaller than or equal to 90 deg.

For bend angles larger than 90 degree, calculating the developed length proves to be a bit more involved.

The general formula of the developed length is: 

L = L1 + L2 - d

With

d = delta value as found in the bend table

b = bend angle  as measured in the image below

L1, L2  = the flange lengths measured to the tangency point.

   

   

 
Fig 1: Parameters needed to calculate the developed length of a bend

The most important aspect to understand in Fig 1 is how the L1 and L2 length values are measured.
They are measured "tangent" to the bend (see also the blue lines in Fig4).

Let's take an example. We start out with a 90 degree flange with L1 = 30 mm and L2 =20 mm (= flange height).

 

Fig 2: Initial 90 degree flange definition

We use a 2 mm bend radius. For that radius we use following bend table in the sheet metal unfold style:

Fig 3: Our bend table definition

We now modify the 90 degree flange to a 95 degree flange.

The most common mistake is to calculate the developed length as

L = L1 + L2 – d = 30 mm + 20 mm – 3.71045 = 46.289 mm

Our L1 and L2 values have changed of course and the L value is incorrect!

Fig 4: Measuring the L2 value

When we measure the L1 and L2 values appropriately, to the tangent line to the bend, filling in the values in the formula is uneventful.

L = L1 + L2 – d = 29.635 + 19.635 – 3.710405 = 45.559595 mm

The calculated result corresponds nicely with what can be measured on the flat pattern

Fig5: Developed length as measured on the flat

Hopefully this gives you an idea on how to reverse engineer Inventor's developed length and assures you a better night sleep, knowing that Inventor does an accurate job in calculating the length J

Bob