Being Inventive

Create linked copies of a Content Center family with different materials using the Material Guide

You want to create copies of a standard family in Content Center.

You want each copy to have a different material.
In addition you want that any change you make to the first copied family will apply to the other copies as well.

In order to achieve this, all copies need to be linked to the first copied family.

So, starting from one standard family and using the Material Guide, you need to create first an independent copy with a different material.

Then, from that family copy, with the Material Guide, create the other copies linked to parent family and assign to each copy a specific material.

You can see the procedure in the video below.

Ale

Create your own Inventor tutorial

I am excited to announce that the Learning Experience (LX) team at Autodesk has published a quick start guide on Autodesk Exchange that explains how to create your own Interactive Tutorial for use in Inventor 2013 and customize the Welcome Screen!!!

What this really means is that ***we just empowered our users to create new content****

When you search for "Inventor tutorial" on Autodesk Exchange, you will see this:

 You can also browse directly to the download locations of the Inventor 2013 Interactive Tutorial Guide App on Autodesk Exchange

• 64bit - http://apps.exchange.autodesk.com/INVNTOR/Detail/Index?id=appstore.exchange.autodesk.com%3ainteractivetutorialguide%3aen

   

• 32bit - http://apps.exchange.autodesk.com/INVNTOR/Detail/Index?id=appstore.exchange.autodesk.com%3ainteractivetutorial-32bit%3aen

   

Click the Free button to download.

The App installs a Quick Start guide, an MP4 video, and two starter templates.

You can provide direct feedback on the App to: learning_app@autodesk.com

Be sure to give the App a review!!!

Thanks

Bob

Inventor 2013 literature for commuters

Our learning experience team has released some interesting new PDF files, posted on the Help wiki.

This is information that was previously available in wiki and chm format but that now can be read at a more leisurely pace as a book on your laptop, PC or tablet.

It might be a good way of spending your time while you are on the go or while you are waiting for the plane, train, bus, taxi or rickshaw.

Here is a summary list of the new PDF.

What's New	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0000-What_s_N0#pageFiles
Inventor tutorials	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0127-Inventor127
Tooling	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0807-Tooling_807#pageFiles
Cable and Harness	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/0904-Cable_an904#pageFiles
Tube and Pipe	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1042-Tube_and1042#pageFiles
Dynamic Simulation	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1111-Dynamic_1111
Stress Analysis	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1163-Stress_A1163
Frame Analysis	http://wikihelp.autodesk.com/Inventor/enu/2013/Help/0126-Tutorial126/1257-Frame_An1257

 

These files are bit awkward to find when browsing the wiki. You will have to scroll all the way down on their respective pages.

Here is an example of the location of the "Inventor Tutorials" PDF in the Files section at the bottom of the page.

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

 

 

 

Cannot embed PDF files in a 64 bit version of Inventor

Please read this new technical article if you experience problems when linking or emdedding PDF files in Inventor.

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

When context help does not show you the right context

I don't know about you but it has frustrated me tremendously in the 2012 release and it continues to be a sore point for me in the 2013 release:
Inventor's wiki Help is not bringing me to where I want to be in the Help. I'll give an example.
When I have the Application Options dialog open on the Drawing tab and I want to know what the Enable background updates option exactly means, I hit the context help icon "?".

Fig 1: Looking for Help on the Enable background updates option …

This brings me to the following wiki Help page.

Fig 2: Application options context help but no sign of Enable background updates option

The problem is that this Help page is collapsed and shows me the top level help for the Application Options.
I want help on an item at a much deeper level than that. Of course I can try to expand several sections in an attempt to find what I was looking for but this is time consuming.
So the reason for my blog post is to show you a much snappier method to get to the context help.

The first step is to avoid the wiki help by downloading the full Inventor 2013 Help and storing it on your local drive.
If you have installed Inventor in C:\Program Files\Autodesk\Inventor 2013, place the local help in the folder C:\Program Files\Autodesk\Inventor 2013\Local Help.

However after doing all this, when you press F1, Inventor still brings you to the wiki.

This is because Inventor's Help reacts differently depending on whether you are connected to the Internet or not

• With internet connection, F1 brings you to http://wikihelp.autodesk.com
• Without internet connection, F1 brings you to the help on your local disk drive

Assuming that most us would not want to give up their Internet connection J, here are the steps to prevent Inventor from searching for the wiki (even if you have a working internet connection).

• locate the file called HelpIds.xml in the Inventor Bin folder (the default location is C:\Program Files\Autodesk\Inventor 2013\Bin)
• Open HelpIds.xml in any text editor
• Search for the section that contains the string "UseOnline"

  <URL

        UseOnline="1"

        Redirect="REDIRECT_"

        OnlinePrefix="http://"

        OnlineWIKI="wikihelp.autodesk.com/?adskContextId="

        OnlineSearchWIKI ="wikihelp.autodesk.com/search?q="

        OnlineSuffix="&amp;language=&amp;release=&amp;product="

        OfflinePrefix="file:///"

        OfflineHelp="Local Help\contexthelp\"

        ErrorPage="Local Help\HELP_INFORMATION"

        OfflineSuffix=".htm"

        />

• Change the UseOnline value from the default 1 to 0.

  <URL

        UseOnline="0"

        Redirect="REDIRECT_"

        OnlinePrefix="http://"

        OnlineWIKI="wikihelp.autodesk.com/?adskContextId="

        OnlineSearchWIKI ="wikihelp.autodesk.com/search?q="

        OnlineSuffix="&amp;language=&amp;release=&amp;product="

        OfflinePrefix="file:///"

        OfflineHelp="Local Help\contexthelp\"

        ErrorPage="Local Help\HELP_INFORMATION"

        OfflineSuffix=".htm"

        />

• Save the xml file

Once the local help kicks in, the context help ends up much closer to where you want to be than with the wiki help.
In my previous example of the Drawing Application Options, you will land in the Drawing Tab section of the Application Option help.

Fig 3: Help shown much closer to the context (before expansion)

It is just a matter of expanding the Capacity/Performance section to see the help on Enable background updates.

Fig 4: Help after expansion

Purists will say that the local help is static and does not benefit from the continuous updates that the wiki help receives.
Personally, I can live with that limitation. I prefer a speedy out-of-date version over a slow up-to-date version.
I know where I can find the latest and greatest Help if need be…

Bob

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