Being Inventive

Controlling include/exclude state of components in Derived Assembly dialog box

When you try to modify the state of Inventor assembly components in the Derived Assembly dialog box, you notice that some components cannot be included or excluded.

The Exclude button (second icon from the left) is grayed out.

This behavior is as designed.

The state (include / exclude) of components in the Bodies tab, depends from the visibility state in the Current Design View Representation if in the Representation tab the “Associative” checkmark is selected.

For example, an occurrence that is invisible is automatically set to the Exclude state and you are no longer able to include it in the derive operation.

To override the default settings and allow inclusion/exclusion of components without any interference of the Design View Representation, clear the “Associative" checkmark on the Representation tab.

This concept is similar to the one explained in this post, when the Visibility context command is disabled in a drawing.

 

In addition to this, in case you want to change the include/exclude state for some components that don’t show at all in the list, check the setting for the Level of Detail in the Representation tab.

In order to show these components in the list and change the include / exclude state, besides clearing the “Associative" checkmark, you need to set the LOD to Master or to another LOD where the components are not suppressed.

Ale

Putting user parameters to work in part sketches in 2013

When I heard about Inventor 2013’s ability to add custom parameters of both text and Boolean types I immediately thought it was a nice enhancement though I couldn’t really see a need to have something like an emboss show “True” or “False” in a part, but there may be a use for Boolean parameters in text that you’ll find and I’m overlooking. The next thought was there had to be a use for a Boolean with the text mixed with a little iLogic.

Here’s a very simple example of using a user text parameter and a Boolean parameter and put them to good use (and add the parameters to a part sketch without getting the “There is no parameter under this source” warning from previous versions)...

The first part is nothing new, just a matter of adding the parameters:

 

Sadly, you can’t send these parameters to a custom iProperty at this point as you can with a numeric parameter by checking on the export parameter box, right clicking and using the custom property format (as in d4 pictured below):

But what a delight to not see the warning when inserting the parameter by selecting the source as user parameters:

Now I can emboss and, voila, it’ll change when I change the parameter - immediately. The possibilities are starting to increase. 

Now the only things left to do are 1) use iLogic to automatically control its visibility (incorporate the Boolean created) and; 2) since I’m already in VB, send the custom parameter to a custom iProperty – after first setting it to a null value so no warnings pop up the first time you run the rule. Why not as long as I’m already there, right? Now the catch here is I can set a string (text) value to null in VB or iLogic, but I don’t know how or if it’s even possible to set a Boolean value to null – just True or False to the best of my knowledge. But we can still use the Boolean to control whether or not the text value is visible with just a few simple lines:

And, now control the visibility of the emboss with that rule and the Boolean parameter:

I hope this helps you find more creative and complex ways to use this new functionality!

-Daren

Refresh material appearance in assembly parts in Inventor 2013

You have changed the appearance of one material and saved the changes to the current active Material Library.

For doing that, you have set, in the active project, the option Use Style Library = Read – Write.

You have opened the Material Browser, for instance, in a part file.

Added the material to the document and displayed it in the editor.

You have applied your modification to the material appearance in the editor.

You have saved the changes in the current active Material Library from menu Manage > Styles and Standards > Save.

After doing that, you open an assembly that contains some components where you had applied the material you have edited afterwards, as explained above, and you want to update the appearance for these components.

In order to do that, in the assembly file, from the menu Manage > Styles and Standards, click on Update.

In the Update Styles dialog, select the active Material Library where you have saved your changes, from the drop-down menu and select the box Update Styles in all Child Documents.

Then, in the menu Manage > Update, click on Update Mass or Rebuild all, for getting the appearance update in the graphic window.

Ale

How to add a spot face symbol to your drawings

We recently issued a hotfix to allow the use of custom fonts in hole notes. Right now the hotfix has been released for the Inventor 2010 Sp4 release only.

Note that thanks to this hotfix, 2010 users now have more powerful hole notes compared to 211, 2012 and 2013 users J.

But they will enjoy this exclusivity not for long. We plan to include the fix in the coming months in the service packs that we will publish for more recent releases.

Let me explain what this hotfix is all about so you understand the extent of its impact.

Without hotfix you are unable to add special symbols or character to a hole note unless you use the AIGDT font via the Character Map icon (see Fig 1).

Fig 1: Adding symbol from the AIGDT font via the Character Map

The AIGDT font suits most special symbol needs in the mechanical drafting arena, except for one particular situation.

It does not include a spot face symbol | SF | according to the ASME-Y14.5M-2009 drafting standard.

The spot face symbol is essential to distinguish a spot face hole from a counter bore hole.

Fig 2: Counter bore and spot face choices

Here is an example of a top view with seemingly two identical holes (if you just look at the hole notes)

Fig 3: Top view of two identical (?) holes

However when creating a section view, the holes look quite different.

 

Fig 4: Section view of the same holes

The hole on the left is a spot face hole and the hole on the right is a counter bore hole.

I admit that I artificially inflated the spot face depth to make it look more dramatic. But you will understand that there is a risk of misinterpreting the drawing by just looking at the top view and when no appropriate symbols are added to the hole notes. Here is where the above mentioned hotfix comes to the rescue. After applying the hotfix you can now select symbols from fonts other than AIGDT. You could even supply your own custom fonts.

If you include the spot face symbol as it can be found in fonts that are freely available on the internet (here is one example ASME-Y14.5M-2009 font), you get this result:

Fig 5: Addition of spot face symbol makes top view unambiguous

The only regret I have in all this is that we were not able to incorporate the same functionality in the style editor. This means that you won't be able to include the spot face symbol in a drawing template and that you will have to add the symbol on an individual note by note basis.

The other element to reckon with is that when you pack and go such a drawing to make sure that you also supply the special font to the party that receives your drawing. Otherwise they would not see the | SF | symbol.

But at least you have the power to create a hole note according to ASME-Y14.5M-2009 without waiting for Inventor to catch up with that standard.

Cheers
Bob

 

 

 

Opening Inventor file opens new instance of Inventor

When you double-click an Inventor part file in Windows Explorer or in Vault Explorer, a new instance of Inventor opens even though the program was already up and running.

This is caused to an improper setting of the following Registry Keys :

HKEY_CLASSES_ROOT\Inventor.PartDocument/SHELL/open/command

Under this key the (Default) value should be showing the path to Inventor.exe with /dde at the end.

The value should be similar to this : C:\program files\Autodesk\InventorVersion\bin\inventor.exe /dde

HKEY_CLASSES_ROOT\Inventor.PartDocument/SHELL/open/ddexec

Under ddeexec, the (Default) string key should be set to: [open("%1")]

This is also valid for the other files types like Assembly which you will find under HKEY_CLASSES_ROOT\Inventor.AssemblyDocument\SHELL\open.

 

Inventor sets automatically these values on Start-up.

So, in order to solve the problem you simply need to log-in as Local Administrator of the machine and start Inventor.

Otherwise, with a Local Administrator user, modify these Registry Keys as explained above.

 

In case, after having applied the steps above, the problem still persists, in the registries, browse to

HKEY_CURRENT_USER\Software\Microsoft\Windows\CurrentVersion\Explorer\FileExts\.ipt

Delete the subfolder “UserChoice” from the above registry branch.

Repeat the procedure for any file type. Change extension as appropriate.

 

Thanks to Pierre Masson for the extensive testing he has done for this solution.

Ale

Creating an ellipse based on its focal points

It has been a while since I have blogged about sketches in Inventor and I thought the new Equation Curve command in Inventor 2013 would be a good occasion to diversify the topics covered on this blog, while at the same time highlighting a cool new feature.

A nice example I can think of is to experiment with ellipses. Inventor generates an ellipse starting from a center point and by defining the extents of the major and minor axis.

But how would you create an ellipse based on its two focal points and the minor axis? It all depends with what Inventor release you are working with.

In 2013:

You can now create an ellipse with two focal points with the new Equation Curve command by using an explicit polar equation. See this part file for an example.

The mathematical definition of such an ellipse based on its two focal points is

r = (B^2)/(A-C*cos(Q))   with Q between 0 and 360 deg

 

Fig 1: Ellipse with half focal distance C shown

A= half major axis

B = half minor axis

C= half the distance between the two focal points

r (radius) and Q(angle) being the polar coordinates of a point on the ellipse (radius and angle)

At the same time A, B and C have to respect the following equation:

A^2 = B^2 + C^2

I have chosen to implement this formula into the parameters dialog:

Fig 2: Parameters dialog takes care of relationship between A, B and C

Note: I added an index 1 to the parameters and used A1, B1 and C1 instead of A, B and C to avoid confusion with reserved parameter keywords.

The result of using such an equation curve can be seen below. The first focal point sits on the origin. To create the second focal point you could for instance mirror the first one along the minor axis.

Fig 3: Creating an ellipse via an explicit polar equation

In 2012 (or earlier versions):

There is not such a thing as equation curves in 2012 unfortunately. But you can quite easily create such an ellipse via the API in the older versions.

You can download here a sample VBA project that you can load in the VBA editor with the Load Project command.

To run the code, run the macro called ShowEllipseDialog

It creates an ellipse with one of its focal points positioned on the origin and the major axis aligned with the X-axis.

You need to have a XY sketch active before running the dialog. The two focal points are connected with a construction line.

B and C values can be freely chosen but A is automatically calculated based on the A^2 = B^2 + C^2 formula.

Fig 4: Creating an ellipse via the Inventor API

Bob

Safety factor of brittle and ductile materials

When working with the Inventor's Stress Analysis module, you have to make a conscious decision whether your material is ductile or brittle.

Inventor will not make this decision for you as this property or classification is not part of the Inventor material properties.

This might be new to some and has led to some interesting discussions on the newsgroup.

Just to be complete, this is not the only decision or assumption to make. There are several other implicit stress analysis assumptions that you make when using Inventor's Stress Analyis software :-)

When assigning materials in the Stress Analysis environment, the Safety Factor column allows you to choose between two calculation methods

Fig 1: Rather subtle choice between brittle and ductile material

What the dialog does not explain is why you would need to make this choice.

The reason is that in order to calculate an accurate safety factor, Inventor uses a different formula depending on the brittleness of the material.

For ductile materials

 

For brittle materials

UTS=Ultimate Tensile Strength (as can be found in the material properties)

For the max. principal stress, we compare the s₁ and s₃ values to account for special combinations of tension, bending, torsion or shear:

Max. principal stress  = s₁                       (if s₃>0) 
                                = s₃                      (if s₁<0)     
                                = s₁- s₃              (in all other cases)

s₁            = 1^st principle stress
s₃            = 3^rd principle stress

It is also important to note that the Max. principal stress is more of a local stress value that has to be measured at the same point where the global maximum Von Mises stress occurs.

The best way to accomplish this is by using the probe tool.

Let's put all this in action with this sample part that contains 3 pressure loads and is clamped down with a fixed constraint on the red face. Skip all existing FEA references on open (I did not attach the calculation results to keep the download size down)

 

Fig 2: Sample part used for the comparison calculations

Case 1: use of a ductile material (steel)

If we activate the first stress analysis in the downloaded part, you will see it has a steel type material with

Yield strength = 260 MPa

UTS = 485 Mpa

Fig 3: Material properties for a ductile material

Make sure to select the Yield Strength calculation for the Safety Factor

Fig 4: Appropriate Safety factor setting for ductile material

After running the stress calculation, we see that the Max. Von Mises stress = 359 Mpa

This means that theoretically

Min. Safety factor = Yield Strength / Max Von Mises stress = 260 MPa/359 MPa = 0.72

This value gets confirmed by looking at the Safety Factor calculation scale.

Fig 5: Safety factors for steel part

 

Case 2: use of a brittle material (glass)

Now let's change the material from steel to glass.

This can easily be done by copying the previous simulation to preserve existing load and boundary conditions.

For your convenience, you can just activate the second simulation that is present in the file.

Assume that we override the steel material and use polished glass with UTS= 50 MPa

Fig 6: Appropriate Safety factor setting for brittle material

 After running the simulation, we want to determine the max. principal stress value.

We first place a probe on the location of the max. Von Mises stress (zoom in to place the probe more precisely).

We then switch to the 1^st principle stress and 3^rd principle stress results and note down the values for s₁ and s₃.

1st principle stress	3rd principle stress

 

s₁ = 258.7 MPa

s₃ = -82.9 MPa

s₁ - s₃ = 258.7 + 82.9 = 341.6 MPa

This means that

Min. safety factor = UTS / Max. principal stress= 50 MPa/341.6 MPa = 0.146

This value gets confirmed by looking at the Safety Factor calculation scale.

Fig 7: Safety factors for glass part 

Needless to say that the glass design (0.15) will break much sooner than the steel design (0.72) …
Enough math for today and let's enjoy the remainder of spring break.

Bob

Export parameters to iProperties as Numeric instead of Text Type

You have exported some parameters of your model to the iProperties Custom tab, selecting the Export Parameter check box.

The Type of the exported parameters in the iProperties is Text by default.

You want to know if there is a way to export them as Numeric Type instead.

In order to do this, in the Parameter list, right-click one of the exported parameters, edit the Custom Property Format and change the Property Type from Text to Number.

Besides, checking the option “Apply to existing comparable parameters” the change will be applied as well to the other parameters of the same type (Length, Volume, and so on), so you don’t need to change the Property Format for each parameter one by one.

Ale

Cannot select target assembly template in Make Components: Selection dialog

You have created a multi-body part.

Then, you go in the Manage tab, Layout and click on Make Components for creating an assembly with components from the solid bodies, but in the following Make Components: Selection dialog, the option for selecting the target assembly template is grayed out.

If you cannot select the Template for the Target assembly, it is because an assembly with the same name exists already in the location where you are saving it.

The behavior is as designed.

For instance, you want to add the components to an existing assembly, as explained in this post.

In this case, you don’t need to select a different template or BOM Structure for the Target assembly.

Instead, in case you want to replace the existing assembly, you have to click the icon for opening the Target assembly folder.

In the following Create dialog, click Yes for creating a new target assembly.

Select the assembly you want to replace.

And accept to replace it.

After that, the option for selecting the Target assembly template will be active.

Otherwise, if you just need to reactivate the option without replacing the existing assembly, you can simply change the Target assembly name in the dialog and the Template selection option will be available again.

Alternatively, you can click the icon for opening the Target assembly folder, in the following Create dialog, click Yes for creating a new target assembly and apply a new name for the Target assembly and / or select a different Target assembly location.

Ale

Dimension of the internal circle of external threads in views

You have applied an external thread to a cylindrical part.

Then, you create the view of this part displaying and dimensioning the thread, but you want to know how Inventor calculates the dimension of the internal circle of the thread.

The calculation is based on the values in Threads.xls file.

For instance you have applied the ANSI Metric M Profile thread (M50x4, Class 6g) to a cylinder with a diameter D = 50 mm.

In this case the diameter d of the internal circle of the thread in the view is calculated with the formula below.

               d = D – [Major Dia Min (column H) – Minor Dia Min (column L)]

That is.

d = 50 mm – [49.465 – 44.642] mm = 45.177 mm

In case you apply a thread and its column L is empty in the Threads.xls file, as, for instance the ANSI Unified Screw Threads and the majority of the Pipe Threads, the diameter d of the internal line of the thread in the view is calculated with the formula below.

d = D – [Major Dia Max (column G) – Minor Dia Max (column K)]

Ale