Dragging in Inventor is Everywhere

In many Inventor command functions you have the opportunity to enter a function value or you can show Inventor the value by left clicking and "dragging" the displayed arrow.  In this article I hope to show you how to make this function as productive as possible.  Below is the extrusion command function that presents a "dragging" value entry.  You would simply left click the arrow and drag to the desired value.

Most all command functions which ask for a value also offer the drag arrow.  The commands cross both modeling and editing functions but depending on your configuration settings, you may not be getting the most from their use.  So I would like to talk about that first.  When I was a machine designer, my CAD manager told me to always design one, to use stock size materials when possible and two, when I had to machine cut material shoot for full inch dimensions, then halves and quarters of an inch.  He made it clear he did not want to see any eights or smaller of an inch unless it was necessary.  Of course we were a high tolerance machine builder and some dimensions had to be in the thousands of an inch and even ten thousands for special fits.  He believed using the largest inch division possible would speed shop production and I must say he was correct.  Just think how sending a piece of structural steel to the saw operator with a non-critical length as 36 47/64 inches instead of 36 3/4 inches would slow him down.  Sure he would probably cheat and round it but you never know.  

The configuration should be done in your companies part and assembly template files so it is available for all designs.  I will be using an inch part template but the same ideas applies to metric templates.  Open up the part template and on the Options panel under the Tools tab select Document Settings.

Select the Modeling tab in the Document Settings dialog box and enter your 3D Snap Spacing for both distance and angle dragging.  This will automatically keep the entry value to increments of the value you enter when you drag a function arrow.  In my case I have set 1/8 inch distance which will quickly give me enough accuracy for non-critical modeling but will also allow me to easily conform to my CAD manager rules just using the drag function, without keyboard entry.

I did not mention it but if you left click and drag on the ball at the base of the arrow, you can "drag" enter angle values in increments of the above setting, in my case 5 degrees.  This is not available in all functions.

Once you have saved your template, your next part or assembly model it will be easy to "drag" the value of your next extrusion, revolution or fillet radius just to mention a few functions.  Of course you can always over-ride the drag value by typing in an value you desire.

So that covers modeling functions but how about sketches.  You can accomplish the same thing in your Inventor sketches by configuring the Snap Spacing under the 2D Sketch section under the Sketch tab in the Document Settings dialog box.  Of course this should also be done in the part and assembly templates.  There is no setting for an increment angle.

There is one more configuration that needs to be set to allow 2D sketch snap spacing to work.  This is done in the Application Options dialog box located on the Options panel under the Tools tab.  On the Sketch tab, place a check mark beside the "Snap to grid" option.  You do not have to turn on the grid display, located in the same dialog box, unless you desire to have a visual grid during sketching.

You will get an odd readout when you are sketching lines at an angle if your Heads-Up-Display Dimension Input is set to "Polar Coordinates".  It is actually snapping to your snap settings but since it is on an angle, the values displayed are not intelligent.  If you change your Dimension Input to "Cartesian Coordinates", the values will display increments of your settings.  I do not believe this is an efficient setting but that is a personal opinion.

So give the Inventor dragging options a try.  If you would like to test before changing your default templates, make the configuration changes in one of your parts using your current template.  If you like them, transfer the settings to your default templates.

Creating a Material Cut List for Your Inventor Drawings

In this article I will be developing a Material Cut List to automatically report cut lengths for common materials used in Inventor.  I will be developing this for one drawing and will not go into the process of editing the project design data and templates to make it available for all drawings.  The process is the same for the most part, only the method of saving the design data will not be covered.  I will be using an Inventor IDW drawing format but the process is identical if your company uses the Inventor DWG drawing format.

Normally cut sizes are applicable to four Inventor standard components.  These are:

• Sheet Metal Flat Sheet Extents
• Content Center Standard Structural Shapes such as angles, channel, and tubing
• Hose lengths either from a routing assembly or lengths used directly in a design
• Pipe and Tubing lengths also from a routing assembly or lengths used directly in a design

Below is my example drawing with one of each standard component.  I have use both a pipe and tube section just to illustrate.  The Material Cut List is the same for both so if you configure for one you will be set for the other automatically.

Keep in mind that the format of the cut lengths and the column headers are fully configurable, you are not restricted to my selections.

The first place to start is to configure your Inventor part template to capture three properties of sheet metal parts, the Sheet Metal Rule which will report to the stock number column, the sheet metal flat pattern width and length.  These configurations are added to your sheet metal template as custom properties.  These custom properties are set to report standard sheet metal properties.  Below I show the custom properties with my chosen names, yours can be anything you desire.  Please note each one is has a function for its value.  SML stands for the sheet metal flat length, SMW the sheet metal flat width and the Sheet Metal Style will report the name of my sheet metal rule which is my material description.  

After selecting an iProperty the value function can be edited using the icon marked with the red arrow.  The initial entry is typed directly into the value box.  The three iProperties and their value functions are:  (the equal sign is a part of the value function.)

• SML  =<Sheet Metal Length>
• SMW =<Sheet Metal Width>
• Sheet Metal Style =<Sheet Metal Rule>

Enter and save these in your Inventor sheet metal template and you are all set.  The Inventor custom iProperty value for structural sections, pipe, hose and tubing are entered automatically during component placement so no modification to your part template is required.  The custom iProperty name for each is listed below.

• Structural Sections - G_L
• Pipe, hose and tubing - PL

The next configuration to to develop a Material Cut List in your Inventor drawing template.  Open up your drawing template and select "Styles Editor" under the Manage tab in the Styles and Standards panel.

Make sure that your are editing your company Design Data standard, expand the "Parts List" entry and right click to on the title to create a new parts list style called Material Cut List.  

Next fill in the title, select the desired text styles and choose other appearance settings to suit your company standards.  The main configuration is to select "Column Chooser" which will allow you to choose what Inventor iProperties to report in the Material Cut List.  

Some of the iProperties are listed in the "Available Properties" table but all custom iProperties are not and you must enter them using the "New Property" icon.  Remember to add the exact custom iProperty name, not what you want the Material Cut List column will eventually read, this is added later.  For example, one of my custom iProperties is PL so this is what I enter in the Define New Property dialog box.

Continue until you  have all the iProperities added then select "OK" to return to the configuration table editor.  You will notice all the selected and entered iProperties are shown in the list.

The next step is to click on each column header and edit the name to whatever value you would like to appear in the finished placed Material Cut List on the drawing.  Keep in mind that names will word wrap if they exceed the column width which is entered in the next column.  You may have to practice with column widths to decide which is best for you.  You can always resize the list after is is placed on the drawing but it is not desirable. 

The next step is to right click on each Property and select "Format Column".  I will start with the Stock Number Property.

The only change I need here is for the Stock Number to report the custom iProperty Sheet Metal Style if it exists.  This is accomplished on the Substitution tab as shown below.

The G_L property has two changes, one to configure the column units format and the value column justification.

The second in to enable value substitution if the component is not a structural component but a pipe, tube or hose.  We would like the PL iPropety value to replace the G_L value if this is the case.  Also you will need to configure the units formatting to use if the substitution occurs.

You will need to configure the last two properties using the Column Format tab to set units display and data justification following the same process used earlier.  When finish, select "Save and Close" to save the changes to the drawing template.  I want again to remind you that I am only configuring the Material Cut List in this drawing, if you are configuring for all drawings, these configuration settings must be exported to the company Inventor design data and template files.

Once you have your drawing view created, you now want to place the Material Cut List.  The placement is accomplished by selecting  "Parts List" command under the Annotate tab and then selecting Material Cut List from the Format drop down.  The process from this point is the same as if you were placing a parts list in the drawing.

One last note, if you have configured your Material Cut List to report sheet metal flat pattern extents you must have developed a flat pattern to have the values populate.  Enjoy!

I Installed the Vault Client, Where is My AutoCAD Vault Add-in Ribbon Tab?

You have installed the Autodesk Vault Client it seems without a hitch.  You open up AutoCAD and the Vault tab is missing.  You scratch your head and wonder what when wrong? 

Take heart, it usually is something very simple.  From this point on, you must be an Administrator of the workstation you are working on.  The first thing to check is if you configured the Vault Client installation to add the Vault Add-in for AutoCAD.  Make sure you close all running programs and go to the Windows Control Panel.  Select "Programs and Features" from the list.  Please note that I have configured my Control Panel for small icons which makes it easier to find.

After the installed Programs and Features have fully loaded, browse down to the Vault Client installation for your version.  In my case I have installed Autodesk Vault Professional 2017 (Client).

Right click on the entry and left click the "Uninstall/Change" option.  Don't worry, you have to choose another option later on if you are uninstalling the application.  Once the application installation routine has loaded, left click the "Add or Remove Features" icon.

The Vault Client feature list will appear.  Look at the list carefully, it represents all the applicable Autodesk applications installed on your workstation that can be configured with the Vault Client Add-in.  In my example, the "AutoCAD 2017 Add-in" is not checked which in turn did not install the necessary AutoCAD Vault Tab.  This could have occurred for two main reasons.  The Autodesk Vault Client was installed "before" the Autodesk AutoCAD application or someone unchecked it during installation.  Left click in the small box to place a check mark.  Select "Update" in the lower right hand corner of the dialog box to continue.  NOTE: If there already is a check mark, skip this step and select "Cancel" at the bottom right side of the dialog box and read on.

Occasionally you will be presented with the following dialog box which is requesting the location of the Vault installation files.  You may have to seek the help of your system administrator as to the files location and then simply use the "Browse" icon to locate it and then press "OK" to continue.

Once the screen informing you that the product was successfully upgraded, select the "Finish" icon to close the application.  Also close the Windows Control Panel.  Next run your AutoCAD application.  Sometimes the Vault Add-in will load up and the Vault tab will appear and you are finished.  If it still does not appear, you have one more step to execute.  Open a new drawing using any template your desire and type "CUILOAD" on the screen and then press "Enter".

This will bring up Load/Unload Customizations dialog box.  The listing at the top are the currently loaded AutoCAD user menus (called customizations).  You will notice that the "Vault" entry is missing.  Select the "Browse" icon at the bottom of the dialog box to continue.

Browse in the folder C:\Users\<current user>\AppData\Roaming\Autodesk\AutoCAD <version>\R<release>\enu\support (normally the default folder) and select the "VaAc.cuix" file.  Select "Open" to continue.

Back in the Load/Unload Customizations dialog box, select the "Load" icon to add it to the Loaded Customization Groups list.  Select "Close" to finish.

At this point, you should have a new "Vault" tab on your AutoCAD ribbon and you are ready to go.

How to Include a Dynamic Part Number in the Part Drawing View Label

There are various methods of detailing machine parts in Inventor.  Some companies use the method of one part per drawing while others desire to place multiple part details on one drawing.  A common practice is to place part detail drawings as sheets under the top level assembly drawing.  When the decision to place multiple part details on one drawing is used, Inventor needs to be configured to place a unique view label for each part to avoid confusion by fabrication personnel.  This view label must also be dynamic so if the part being detailed is changed, the view label will update to reflect the new part information.  Below is an example of this type of drawing showing view labels containing the part number of each placed part.  The configuration of Inventor to place a dynamic view label, containing the part number, is the focus of this article.

The process beginnings with the editing of the drawing template and the controlling Design Data, sometimes referred to as the Styles Library.  This article will not go over the process of creating a set of Inventor templates and their matching Design Data but it will cover the drawing style configuration, contained in the template, to accomplish our goal.  A drawing template is configured to follow a defined Active Standard as shown in the Document Settings dialog below.  If you open one of your Inventor drawings and choose Document Settings on the Tools tab under the Options panel, you will see the this active standard.  It is coming from the Design Data folder which is defined either in the Inventor Project File or in the Applications Options.

For demonstration, I will be modifying the Design Data for a single demo drawing which will not be permanent for all future drawings.  To make it a permanent setting, the Design Data library must be edited.  For this one drawing I select the Styles Editor command which can be found under the Manage tab on the Styles and Standards panel.

In the Styles and Editor dialog box, I select my Standard then the View Preferences tab.  Notice that the editor is in Read Only mode since I am only editing this one drawing.  

The View Label Defaults is the area where I can configure the information that will be included in my base view label.  The first thing I will set is which model property will be displayed in the view label.  In the Display panel you will notice the standard Inventor view label configuration.  Selecting the "pencil" icon will display the following dialog box.  Follow the numbered steps to replace the default <VIEW> entry with the model property "Part Number".  Select "OK" to finish.

Next I will leave the View Type on "Base" since I want the view label to be automatically placed  on the base view of each part.  Last I will choose the position of the view label and select the Visibility icon to make the bulb "light" indicating that the view label will be displayed.  I finish by selecting Save to exit the Styles Editor.

When I place the base view of my part along with any projected views and select OK the view label appears under the base view.  At this point you can drag the view label to a different position if desired.  If the base view is moved, the label will follow it.

If I wanted to add "PART NUMBER" to the label entry, I simply add it as text in the Display dialog box.

To prove this part number is dynamic, I will use the "Replace Model Reference" command to replace the part in the drawing view.  This command is located on the Modify panel under the Manage Tab while in the drawing.

As you can see, if this modification was made to the Design Data library for all drawings it will make the management of multiple part drawings a lot easier.