Saturday, January 15, 2011

Use iLogic to fill out your title-block name and date

You have a Drawn By: and a Date: field in your title-block, but it's difficult to remember to edit the iProperties when saving the file, or rolling the revision, etc.

Create an iLogic rule to write the User Name ( pulled from Application Options > General tab ) and the current date to the iProperties. You can then set your title block fields to read those iProperties. And then finally set the rule to be triggered using the Before Save Document event trigger so that the title-block is always updated at the time of the file save. (Ribbon: Manage tab > iLogic panel > Event Triggers)

Here is an example snippet, where the user's name is written to the Author iProperty and =Now is used to write the date to the Creation Date iProperty. In this case the If statement is used to check to see if the Author value matches the UserName, if not it sets it to match, then displays a message box. You'll note the message box title uses the UserName to personalize the message:

myName= ThisApplication.GeneralOptions.UserName

If iProperties.Value("Summary", "Author") <> myName Then
iProperties.Value("Summary", "Author") = myName
MessageBox.Show("The Title block has been updated","an iLogic message for: " & myName)
End If

iProperties.Value("Project", "Creation Date") = Now

Tuesday, January 4, 2011

Autodesk Inventor Perfect Spacing Everytime

Here's a quick video tip on letting Inventor do the math for you when you need even spacing in a sketch.

Note: the actual video quality is better than this thumbnail preview appears.
Inventor Video

Now Here's A Good Book

I could ramble on with a wordy review, but you'd probably just click the link and check out what others have to say about it anyway right?

If you do design work you should have a look, enough said.

by Rob Thompson

iLogic Code To Set The Part Number Per Length Range

You purchase stock lengths of material, and then cut them to length. You want to assign a part number based upon the part length so that if the part falls into a given range it receives one part number, and if it falls into another range it receives a different part number, and so on. Thus assigning part numbers based on the stock material lengths.

    Click to Enlarge
  • First a multi-value parameter is created and the stock sizes are added to the list, in this case the list is a user parameter called Size. 
  • Next an iLogic rule is created, and an input box is set to read the multi-value list, so the user can select one of the stock sizes.
  • Then a model parameter called Length is set to equal the user parameter called Size.
  • The part is updated to reflect the parameter change
  • A conditional if/then evaluates the length parameter and sets the part number iProperty based on the Length of the part.
  • And finally a message box displays the assigned part number for confirmation.
'get size from list
Size= InputListBox("Choose Size", MultiValue.List("Size"), _
Size, Title := "Select Size", ListName := "Available Sizes")

'set length to be Size
Length = Size

'update the part to reflect the parameter change
iLogicVb.UpdateWhenDone = True

If Length <= 250 Then
iProperties.Value("Project", "Part Number") = "000-10"
Else If Length <= 500 Then
iProperties.Value("Project", "Part Number") = "000-20"
iProperties.Value("Project", "Part Number") = "000-30"
End If

'evaluates the length parameter and sets the part number iProperty
PN =iProperties.Value("Project", "Part Number")

'displays the Partn number in a message box.
MessageBox.Show("Part Number: " & PN, "Part Number Confirm",MessageBoxButtons.OK)

 This shows the rule in action, with the part number range scale sketched for illustration purposes. If the length is 250 or less then the part number is 000-10, if its over 250 and less than or equal to 500, then it is 000-20, for anything over 500 the part number is 000-30.

Click to Enlarge
Click here to download the example file (Inventor 2011)
The file is called PN Range From List.ipt

Look for more iLogic examples on this blog or in the chapter dedicated to iLogic Basics in the next edition of Mastering Autodesk Inventor book (due out in June of 2011 if all goes well). 


Off Topic, But Fun.

Gymkhana Video


Gymkhana is a type of motorsport practiced in an increasing number of countries. Similar to autocross, gymkhana courses are often very complex and memorizing the course is a significant part of achieving a fast time. More From Wikipedia Here

3D Intersection Curve

You want to create a sketch along a 3D surface where it intersects another 3D curve.

Use the 3D Intersection tool to do this in a 3D sketch. See this video. Not too this is covered in Chapter 3 in the 3D sketching pages, of the Mastering Inventor book.

Inventor Video

Autodesk Install or Licensing Problem?

If you have an install or licensing question you can search existing questions or post a new question on the: Installation & Licensing Discussion Group

Don't forget to provide as much detail as you can about operating systems, Inventor versions, and things you've tried up to this point. 

Feature Request For Inventor

Have an idea for a feature enhancement or a new tool you'd like to see included in Inventor?

How about an Inventor Easy button?

Use this Autodesk Feedback link to tell them about it.

Or use this new link for the Inventor IdeaStation .

Keep in mind that Inventor's development team actively works on future releases of Inventor well in advance of the release date, so the improvements for the next release of Inventor have most likely already been decided. But the feedback will be considered in the development cycle as you submit it.

Contact Solver

You want to setup your Inventor assembly so that parts will not pass through each other in an unrealistic manner.

Add components to a Contact Set and then use the Contact Solver tool to allow Inventor to solve for contact. See video for how the tools work.

Note: It’s best to disable this feature when not specifically testing part contact, as it may impact performance in a negative way as Inventor attempts to solve contact relationships as you drag parts around in typical constraint and assembly tasks.

Inventor Video

Graphics Issues – Application Options Setting - Use Software Graphics

You’re having graphics issues in Inventor, but you’re not sure if it’s the graphics card or some other problem.

Go to Tools tab > Application Options > Hardware tab, and select the setting to use the Software Graphics. Then close and re-open the file to let Inventor.

This setting uses Inventor to render the onscreen graphics and therefore any graphics anomalies that exist while using this setting can be attributed to something other than the graphics card. If the issue returns when you set the option back to the recommended setting, then you should look into updating or rolling back your graphics card driver, or getting a different graphics card that handles Inventor graphic better.

Keep in mind this is a just a test, and it is not recommended to run Inventor all of the time using the Software setting, as it will cause Inventor to run slowly.

ALT + Drag Assembly Constraints

In past versions of  Inventor you used the ALT + Drag method to create assembly constraints, and employed keyboard shortcuts to allow you to change the constraint type. But now when you try it the ALT key highlights the Ribbon Keytips* as shown below, and does not allow you to enter the keyboard short cut to change the constraint type.

When you see the Ribbon Keytips appear, let up on the ALT key and then press the ALT key again.

You can drag a component into position and automatically place a constraint (with no offset) by following these steps
   1. Hold down ALT, and then click the component to drag.
   2. Drag the component into position. As the dragged component nears the target component, the constraint is previewed.
   3. When the component is in the appropriate position, release the mouse to place the constraint. 

The type and solution of constraint you get depends on the geometry selected. For instance, when you drag a cylindrical part over another cylindrical part or hole, an inferred Mate constraint along the axes results. If you position the dragged part over a component face, Inventor infers a mate between planar faces.

   4. Change the constraint type by letting up on the ALT key and then pressing the ALT key again, then use one of these keyboard shortcuts:

M or 1 Changes to a mate constraint.
A or 2 Changes to an angle constraint.
T or 3 Changes to a tangent constraint.
I or 4 Changes to an insert constraint.
R or 5 Changes to a rotation motion constraint.
S or 6 Changes to a translation (slide) motion constraint.
X or 8 Changes to a transitional constraint.

The constraint glyph will change to indicate the current constraint type. If the geometry does not allow for one of the constraint types that Keyboard short cut is not offered.

*What are Keytips?
  • Use the keyboard to access the Application Menu, Quick Access toolbar, and ribbon. 
  • Press the Alt key or F10 to display shortcut keys for common tools in the application window. Keytips allow you to perform tasks without using your mouse. 
  • When you select a keytip, more keytips are displayed for that tool. Keytips appear as underlined characters to indicate which key or combination of keys on the keyboard must be pressed to activate a command.

Keytips allow you to navigate in the Application Menu and in the ribbon using only the keyboard. Use the keyboard arrows to navigate to commands on the ribbon and Application Menu

Note: Keytips are not customizable.

How to get imported parts and surfaces to show up in a drawing view?

You’ve imported a file (such as STEP or IGES file) but it has come in as a surface model rather than a solid. Because your needs don’t require the file be made a solid, you decide to use the file as is, rather than taking the time to repair it to get it to a solid. The problem is it won’t show up in the drawing view.

In the drawing, expand the view node in the browser and locate the model node, then right-click and choose “Include All Surfaces”.

If the surface is a work surface in a part, you'll right-click on the top level of the part node:

If it is a surface based part in an assembly, you'll right-click on the the part node in the assembly tree:

Missing Dialog Box in Autodesk Inventor?

You try to use a tool in Inventor, but nothing seems to happen, and you can’t click anything else. If you press the ESC key, then everything is okay. But it happens again if you try to use that particular tool.

Most likely the dialog box for the tool you are trying to use is coming up off screen. This often happens when a configuration for dual monitors has changed. To resolve this:

  • start the tool that exhibits the problem
  • press ALT + Space-bar on the keyboard 
  • then press the M key (M for move)
This is what happens off screen

  • then Immediately press any of the arrow keys on the keyboard
  • finally, move your mouse around and the dialog box will now be attached to your cursor allowing you to drag it back on screen, just click to drop it in place.

To see this in action you can try it with a dialog that does come up on screen and follow the steps above.