IMAGINiT Manufacturing Solutions Blog

Sketch Object Properties

When creating advanced or complex Inventor sketch profiles, it is sometimes helpful to change the display properties of the sketch geometry. Inventor provides some basic options for this … Center Lines, Construction Lines, Reference (Projected) Geometry, and Normal Geometry. Under most conditions these options are all you need, however when you build sketches that will be shared, or used as layout information in skeleton modeling, having visual clues to what the geometry represents can be helpful (think AutoCAD Layers).

To access and set the properties of objects (lines, arcs, circles) in a sketch you have several options available to you.

Tool bar access via a Drop-Down menu

Right Click on either the Sketch in the Browser or on the individual objects and select Properties from the menu.

Work Flow

In this example we have several sketch profiles defined in shared sketch. To make it easier for other users to visualize the different profile information we will change the color and line styles of the objects in the sketch.

Starting with the rectangle on the left, we select the 4 lines, then right mouse click to select “Properties”. In this example the Color, Line type and Line Weight were adjusted.

In the next example we will display the bolt circle as a center line. Currently the Inventor Center Line sketch style does not support Circles or Arcs. In this example an additional change was added by activating Scale to control the size of the displayed Line Style.

Now that we have adjusted the visual characteristics of the sketch it is easier for the end user to determine the purpose and relationships of the different objects.

After setting the display characteristics of the sketch objects, you can toggle the display using the “Show Format” option from the ribbon bar.

Passing Model iProperties to Drawing iProperties

During the documentation process, we often use the same iProperties from our modeling files (parts & assemblies) to populate fields in our Bill of Materials, Parts Lists, drawing Title Blocks and Vault.

When we create a drawing, we often find ourselves re-entering the same data for the drawing’s iProperties that we entered for documented model’s iProperties.

For our drawing Title Blocks, this duplicated effort can be removed by mapping the Title Block fields to get iProperty data from the model. However, this solution still leaves the drawing iProperties empty.

Inventor does provide a solution for this from the Document Setting where we can configure the drawing to use the iProperties of the model.

Workflow

Start a new file or open one of your drawing templates files, navigate to Tools, and select Document Settings.

On the Document Settings Dialog, select the Drawing Tab and then select “Copy Model Properties”

Enable the functionality by selecting “Copy Model Properties” and then select the required properties that to be copied from the model.

Save your template file back to your template directory. When you create the first base view of a new drawing, the selected iProperties will update with the corresponding values from the model file.

Note: Any edits to existing values in the model’s iProperties will not update the drawing iProperties after the base view is created.

Saving Inventor CAM Stock for Secondary Operations

Creating a stock setup with Inventor CAM is simple if you’re starting from stock that’s cylindrical, box, or tube shaped. But what if your part has been pre-machined for tooling, cast, or has a complex shape? Inventor CAM equips users with the ability to save the stock body at any stage in the machining process and then use it in secondary setups!

Take a look at the part below. The initial roughing and internal boring is done by turning down the part on a 2-Axis lathe. This will leave the subsequent milling, chamfer, and drilling operations to be done with a vertical mill.

To export the remaining stock for the milling setup, follow these steps:

1. Run the toolpath simulation until it’s finished.

2. Right-click anywhere in the graphics window and select Stock > Save Stock.

3. Choose a folder location to save the stock body. Give the file a unique name that represents the first set of operations. The file type will default to Stereolithography (.stl) format.

4. Select "Save."

5. From the “Manage” tab – click on “Import.”

6. Navigate to the folder where the stock file was saved and select it.

7. IMPORTANT! Before selecting “Open” – click on “Options.” Set the Import Units value to “millimeter.” This assures that the .stl file is converted correctly. If this step isn’t taken – the body will be about 25 times too big.

8. Select “Open” to import the stock solid to the part file.

9. The STL body should automatically be imported and located in the same orientation as the model body. It will appear as a black triangulated geometry. In the model browser you’ll see it labeled as a “MeshFeature.”

 

10. From the CAM tab on the Job panel select “Setup.” to create a new stock setup for the remaining vertical milling operations.

11. On the “Stock” tab, change the Mode to “Stock Solid” using the drop-down menu.

12. Click on the black STL body as the Stock solid. It should highlight the surface in yellow.

13. On the “Setup” tab – select a new Stock WCS point and orientation for the milling setup. Typically this will mean the Z-axis will be specified as the vertical milling direction.

14. Return to the model browser and right-click on the mesh body. Select “Visibility” to hide the body.

15. Add the required 2D and 3D milling toolpaths to finish the machining program. Simulate the second setup to visualize the final stock removal.

NOTE: The same process can be used to import modeled stock solids (e.g. cast or pre-machined parts). A variety of formats besides STL are accepted including STEP, IGES, and Parasolid files.

 

There's a property for that

Articles and videos of new features are good for providing awareness, but they don't always answer the question "So what?"  That's why I like real world examples that actually show their value.  Here's an example a customer recently had where one simple feature was able to save hours of tedious analysis.  The feature?  The property Has Drawing that made its appearance in Vault 2020 (at the time, 2020 was the latest release, so it was still a new feature).  An idea that had been around for a few years that was actually green-lit into the product.

Scenario: Customer utilized custom material libraries for their parts.  Some of those materials didn't have precise names, which was fine when they only had single source suppliers with which they had a shared vocabulary; each knew what those material names meant.  Once designed, parts were documented with material names in the notes.  The material property is mapped into Vault so that it is searchable, though, not editable in Vault.

Problem: A change in business required them to utilize more than one supplier, but the material names remained the same.  Again the names were descriptive, but not precise.  So they were getting varying results when the parts came in from the different suppliers.  It was then decided to change the material names so that parts could be fabricated consistently.  But that meant changing hundreds of drawings.  And to make matters worse, not every part was documented in a drawing.

Solution: They could easily enough search the Vault for all the parts that had material names that required changes.  However, they only really needed (at the beginning stage) to change the drawings, as they were the deliverable to suppliers, not the native part files.  They would have had to analyze thousands of parts to see which had drawings and which didn't.  We set them up with the "Saved Search" seen below.

Results: The saved search, utilizing a parametric material search condition gave them the flexibility to search for an offending material and get a "punch list" of the parts that had to be changed.  Once the material was changed they were able to just update the drawings by using the handy Open Drawing from Vault command in Inventor.

Managing Styles and Standards in Autodesk Inventor

Introduction

Styles and Standards are, and always have been, a sticking point for a lot of Inventor users. The complexity of managing them seems to be far more involved than required. But once you understand how styles are managed it becomes a very good way to ensure consistency across your design team.

In this guide I hope to explain how Styles are managed by inventor both inside the active document and externally by Style Libraries, and how users can interact with Styles and Standards to improve efficiency in the workplace.

What are Styles and Standards?

Let us start with a brief description of what styles are in the context of inventor. Most commonly people know that Styles are used to control the appearance of annotations, tables, text, etc. in the drawing environment. However, they are also used to control things like sheet metal rules, unfold calculations and lighting.

Standards are used in the drafting environment and define a collection of styles that create the Company/Project “Standard” for drawings. What these means is that all the designers are working with the same styles when creating drawings which ensures consistency across documentation.

Figure 1 - Style and Standard Panel

The Style Editor in the ‘Styles and Standards’ Panel of the ‘Manage’ ribbon tab (Figure 1) is used to create, modify and delete styles and Standards. The style editor dialog box appears differently depending on the environment in which you open it. From a part, assembly or weldment file the style manager only shows the lighting and text styles. From a sheet metal part, the style library shows the lighting, sheet metal rules, Sheet metal Unfold and text styles. And from the drawing environment the style manager shows all annotation styles including text, tables, dimensions, etc. and two important Style Types:

• Standards
• Object Defaults.

Most commonly people manipulate styles in the drawing environment so that is what we will focus on in this article. (Figure 2)

Figure 2 - Style Manager (Drawing Environment)

What's a Style Library?

A Style Library is a collection of external .xml files that contain Inventor styles. Each .xml file controls a ‘Style Type’ such as ‘Dimension’ or ‘Table’. If you have only one Style Library, it is commonly referred to as the Global Style Library as it contains all the styles provided by Autodesk® as well as any you create and save to it. It is highly recommended that all companies with multiple users have a common Design Data folder either in the Vault or on a network location that all Inventor users have access to. This allows consistency across the department by ensuring everyone is working with the same design data. With a default install of Inventor, the Global Style Library is located in the following area:

C:\Users\Public\Documents\Autodesk\Inventor <Version>\Design Data

Note: It is possible to have Project specific Style Libraries however, for the purposes of this article, we will only consider the Global Style Library 

What is the Relationship Between Style, Standards and Style Libraries?

This is where things get more complicated. Even though every document has access to the Global Style Library the document only loads the styles into the document that are specified in the ‘Standard’. What this means is that each document embeds the styles specified by the Standard into the file creating, in essence, a Local Style Library. And this is the crux of the issue when it comes to managing styles. When a user modifies/creates a style, it is only created/modified in the Local Style Library. There is no persistent connection between the styles embedded in the file (the Local Style Library) and those in the Global Style Library.

What Happens When You Change a Style in a Drawing?

Consider the following workflow as an example of editing a style in a drawing:

1. Create a new Drawing document from a template
   
2. Place base, side and top views and position accordingly
   
3. Dimension the views
   
4. The user decides the dimensional precision is to loose and changes the [Default-mm (ANSI)] dimension style (the dimension style specified in the Default-mm (ANSI) Standard that is currently active) to increase the precision from 2 decimal places to 3 decimal places
   
5. All dimensions that are of the [Default-mm (ANSI)] dimension style are updated automatically and now show a precision of 3 decimal places.
   

Note: At this point the User is modifying an existing dimension style here not creating a new one – this will become important later.

As discussed earlier the change this user has made is only affecting the Local definition of the [Default-mm (ANSI)] style that is embedded in the file. Hence, if this user now created a new drawing from the same template file the precision setting would be reset to two decimal places. This is because the [Default-mm (ANSI)] style is loaded from the Global Style Library upon creation* of the new document and the Global Style Library definition of this style has a precision setting of 2 decimal places.

*In reality, the Template files already contain the styles from when they were created and if the styles match nothing happens. If there are styles that do not match, however, Inventor will automatically update the Local Styles to match the Global Styles. This is often seen in the ‘Style Conflict’ message as shown in Figure 8. This will be addressed later in the document.

Figure 8 - Style Conflict Message Box

How Do You Make Changes to a Style Library?

Making a change to a library involves saving the Local Style changes to the Global Style Library. If the style is new it creates a new style in the Global Library and if it is modified it overwrites the existing style in the Global Style Library. Consider the workflow just demonstrated, the following example works through the process of updating the Global Style Library:

1. Select the ‘Save’ button on the ‘Styles and Standards’ panel of the ‘Manage’ Tab
   
2. In the ‘Save Styles to Style Library’ dialog box, click the ‘No’ under the ‘Save to Library’ column to toggle it to ‘Yes’
   
3. Click ‘OK’
4. Click 'Yes’ to the warning dialog box
   
   Note: This will overwrite the style definition in the Global Style Library and so, before making any edits, it is recommended you make a backup of the Design Data folder incase anything files becomes corrupted/unusable
   
   
5. That’s it. The style has now been overwritten in the Global Style Library and every new drawing created that uses the [Default-mm (ANSI)] dimension style will, by default, have a precision of 3 decimal places.

Some caveats for this process:

• The Style-Library setting in the Project file must be set to Read-Write
• You must have ample permissions to overwrite the .xml files in the Design Data folder
• If utilizing the Vault to manage data, you will need to check out the .xml files in order to make the changes
• Now the Global Style Library has been updated the ‘Style Conflict’ message will appear every time a user creates a new file from a template.

Now we know the process let’s examine the ‘Save Style to Style Library’ dialog box in Figure 10.

This dialog box is displaying the following:

Column Name	Description	Example
Document Name	The file in which the new/modified Style is embedded	Style example.idw
Style Name	The name of the style that has been created/modified	Default-mm (ANSI)
Type	The Type of style that has been created/modified	Dimension
Location	Whether the Style exists ‘Local’ (embedded), ‘Library’ (external) or ‘Both’	Both
Change	Whether the style was changed in the document or in the library*	Local
Save to Style Library	Toggles between ‘Yes’ and ‘No’ to indicate if the user wants to save the style to the Library or not	No**

*If the Style is new and not in the Global Style Library this shows up as ‘No’
**This was changed during the above workflow to ‘Yes’ as an example of saving a style to a library

How Can an Old Drawing be Updated to the Current Standard?

So, we have successfully changed the [Default-mm (ANSI)] style and saved it to the Global Style Library, but now we have opened and old drawing and none of the dimensions are displayed at the new standard despite their Style showing as [Default-mm (ANSI)]. Again, this is due to there being no persistent link between the embedded styles and the Global Style Library. So, in order to update the drawing to match the latest Styles and Standards we must use the ‘Update” command on the ‘Styles and Standards’ panel of the ‘Manage’ ribbon tab.

Upon selecting the ‘Update’ command an ‘Update Styles’ dialog box appears (Figure 12)

Figure 12 - Update Styles Dialog Box

Note how similar this appears to the ‘Save Styles to Style Library’ dialog box. That is why it is important to take note of the dialog box you are working with prior to selecting ‘OK’. The dialog box contains all the same columns, except for one, as the ‘Save Styles to Style Library’ dialog box. The one column difference is the last column where it says ‘Update’ instead of ‘Save to Library’.

When you have selected the Styles you want to update to the current standard select ‘OK’ and you are presented with a message box (Figure 13)

Figure 13 - Update Message Box

This informs the user that any locally edited styles will be overwritten with the Global Style Library definition effectively erasing any of the edits. However, unlike saving styles to the Global Style Library, this process can be undone. If you make an error in your selection you can always undone the command and go back to select the right styles to update.

A Graphical Representation of Styles and Style Libraries

Figure 14 - Graphical Representation of Style Management

Understanding Standards

We have delved into Styles and how they are managed between documents but that is only part of the problem when it comes to effective use of Styles in Inventor. Now we need to understand how styles are managed in the documents and that is done using Standards.

Note: Standards are only available in the drafting environment

When you open the Style and Standard Editor the first category in the left-hand pane is Standard. This is where we can see what Standards are available to us and “Activate” the Standard we want to use. When you Activate a Standard, you are defining what styles are available to the user during drafting. You can tell which is the Active Standard as it is highlighted in Bold. See Figure 15.

Figure 15 - Standard Categories

When you select a Standard to edit, see Figure 16, the right-hand pane consists of 5 tabs:

• General
• View Preferences
• Available Styles
• Object defaults
• And Material Hatch Patter Defaults

Figure 16 - Styles and Standards Editor (Standards)

The General Tab contains settings for the Units, decimal marker, Character Exclusions, etc. The View Preferences Tab contains settings for default view labels, how sections are details, First/Third angle projection, etc. And the Material Hatch Pattern Defaults is just that, here you can set up the default hatch pattern for set materials when sectioning them in drawings. The two tabs that we are going to discuss in more detail are the ‘Available Styles’ tab and the ‘Object Defaults’ tab.

Available Styles

The ‘Available Styles’ tab is where we can specify what Styles should be made available, when the standards is Active, to the user.

Figure 17 - Available Styles Tab

As you can see from Figure 17 there are 5 Dimensional Styles available that can be checked. There are also 18 Style Types to choose from, each with their own list of Available Styles. When a Style is Checked in this box and while the Standard is Active, that style will be available to to use in the Document. An important thing to note here is the Style Filter in the top right of the Style and Standard Editor dialog box (Figure 18).

Figure 18 - Style Filter

This filter allows us to control what shows up in the Editor dialog box. There are three options available to use:

• Active Standard
• Local Styles
• All styles

This filter allows us to narrow down large amounts of styles (All Styles) to just ones contained in the document (Local Style) or currently available in the Active Standard (Active Standard). See Figure 19 and compare this to Figure 17 for an example of how the available Styles and Standards Editor dialog box changes when the user sets the filter to All Styles

Figure 19 - Available Styles (All Styles)

When you are creating a new style the dialog box allows you to automatically add that style to the Active Standard as shown in Figure 20.

Figure 20 - New Local Style dialog box

Object Defaults

An Object Default sets the default style and layer for each object type in the drafting environment. As an example in the Objects Default tab of the Default Standard (ANSI-mm) the Object Type “Linear Dimension” has an Object Style specified as [Default – mm (ANSI)] and a Layer Specified as [Dimensions (ANSI)]. See Figure 21

This means that when the user places a linear dimension it will be placed on the [Dimensions (ANSI)] layer and its appearance will be defined by the [Default – mm (ANSI)] style.

Figure 21 - Object Defaults Tab

Figure 22 - Object Defaults Edit

This tab, however, does not allow you to edit the Object Defaults directly. This tab allows the user to select an Object Defaults Style in the Active Object Defaults dropdown box above the window which will be applied to the active standard. From here the user can also select the pencil which will redirect to the referenced Object Default Style for editing as shown in Figure 22

Form here the user can define what the Object Style Default and Layer Default should be and create a new Object Default Styles for reference by the Standard rather than modifying an existing one.

Purging Styles

The last item we are going to touch on in this article is the purging of styles. The Purge command is the last command located on the ‘Styles and Standards’ panel of the ‘Manage’ ribbon tab.

Figure 23 - Styles and Standards panel

The Purge command clears any unused styles, materials and appearances from the document. This allows the user to remove any unwanted data that is taking up space in the file and helps improve clarity when managing styles, materials and appearances. It is important to note how the program only selects styles that can be purged.

Firstly, the style must not be in use. If the user has a dimension placed that references a particular style that style is in use and cannot be purged. Moreover, if the style has been made “Available” in the Standard it is also considered “in use” and cannot be purged.

Secondly, the command only purges styles that are embedded in the file (Local). So, the command is safe to use knowing that any Style in the Style Library is safe from being purged.

Figure 24 shows the available ‘Dimension’ Type Styles in the [Default Standard (ANSI)] Standard. This list has been filtered to only show the “Active Standard”. You can see, due to the filter in place, all the dimension styles are checked.

Figure 25 shows the same list with the results being filtered to “Local Styles”. Notice there are now 3 additional Styles in the list that do not have checks against them. This tells us that the document has 3 additional ‘Dimension’ Type Styles embedded. If these styles are not in use the file is larger than it needs to be, and it is less clear what Styles are currently in use and available.

These styles are not part of the Active Standard however, they might still be in use in the document and hence not capable of being Purged.

Figure 24 - Available Styles (Active Standard Filter)

Figure 25 - Available Styles (Local Styles Filter)

Below is an example of the Purge workflow:

1. Select the Purge command on the ‘Styles and Standards’ panel or the ‘Manage’ ribbon tab
2. The ‘Purge Styles’ Dialog box is displayed
   

   Figure 26 - Purge Styles Dialog Box

3. The ‘Purge Styles’ Dialog Box resembles both the save and update dialog boxes displaying the same information.
4. Click on the ‘Yes’/’No’ in the Purge column to toggle if you want the style to be purged or not.
5. Once the Selection is made click ‘OK’
6. The Styles have been Purged.

Manual Management

The commands demonstrated in these workflows are used to highlight Styles and Standards that are new, updated or unused and deal with them accordingly. If you have a particular Style that you need to Save, update or Purge this can be managed manually in the Styles and Standards Editor through the use of the shortcut menu using a right click (Figure 27). Using this method the user can purge styles that are currently referenced by the active standard, however, if you try to Purge a Style that is referenced by the Active Standard Inventor will warn you that the Standard will be modified to reflect this change (Figure 28). This means the Style will be removed and the standard will be updated to remove that Style from the Available Styles List.

You should never attempt to manage Style Libraries through the use of an .xml editor. Only use the tools provided by Autodesk to make edits to the Style Library.

Figure 27 - Manual Style Management

Figure 28 - Purge Local Style Dialog Box

Conclusion

Styles, Standards and Style Libraries can be confusing when first trying to understand the relationships between them. It is well worth spending the time to learn and understand this relationship as having a consistent Standard across the company not only provides a professional appearance to your documentation, it also makes production of these documents consistent and more efficient for the design team.

This article has been designed to give the reader a high-level overview of the Styles, Standards and Style Library relationship and an introduction into the tools that can be used to manage them. These tools are sufficient to get a Standard in place and manage that Standard and associated Styles. However there is a lot more information about styles available and, if you are managing company drafting standards, time should be spent understanding styles in more detail.

Fusion 360 Title Blocks

Fusion 360 (Fusion) has 2 basic workflows for creating custom Title Blocks.  The first is to create the Title Block within Fusion and the second is to create the Title Block in AutoCAD and import it into Fusion.  The first option (Create within Fusion) is pretty straight forward and the way to go if you do not have or know how to use AutoCAD.  The second (Create in AutoCAD) is for those of us who have and are comfortable using AutoCAD.  Lets take a look at both.  NOTE: This is not a tutorial on how to draw in Fusion or AutoCAD but, just how the Title Blocks works.

To get started with either option the process is the same.  Follow these Steps.

1. Optional, but recommended is to have a Project that contains your templates and other company standards.  It is also, recommended to sketch out on a piece of paper what you want the Title Block to look like, and what information is required and what information is optional before you begin.
2. Start a New Drawing Template.
   
   • 

   • Select "From Scratch" and choose the standard, units, and paper size.

     • 

   • At the bottom of the screen select "Add Title Block"

     • 

   • You now are presented with 3 options.

     • 
       
       1. From Existing

          • Create Title Block from an existing one

       2. From Scratch

          • Create a brand new Title Block from scratch

       3. From DWG File

          • Import from an AutoCAD DWG

Option 1 - Fusion 360

1. Select Option 2 (from above) and give your Title Block a name
   • 
     

2. Fusion will give you basic drawing and modifying tools (Geometry and Modify Panels) to design the Title Block. 

   • 

   • Attributes (Text Panel) are very easy to place with the built in attribute names already populated (7 built in attributes) .  If you require more information than the 7 provided, you can also easily place custom attributes to add additional data.

     • 
   • Fusion attributes and where they are pulled from are listed below.  Most of the attributes are read only once when the drawing is created so, if you change the model's title, project…, the attribute value will not update automatically. You will need to modify the Title Blocks attributes manually by double clicking on the individual attribute(s). (insert sad face).  Filling out custom attributes is done by simply double clicking on the attribute in the Title Block.

     • TITLE_1

       • This pulls the name you saved the Fusion file with.

     • SHEET

       • This will add the sheet number and total sheet count (1/3, 2/3, 3/3…. In this format)

     • PROJECT
       • When you save your file, it is saved within a project folder.  This will pull the project folder name.  So, be thoughtful how you organize your data and if you want all CAPS you need to type in your project folder name with all CAPS.
     • SIZE

       • This will pull in the sheet size of the template.

     • SCALE
       • This will pull in the scale of the first view and how you typed in the scale (1:1, 1/1, 1…).  Also, if you change the scale after the first view has been placed, and you want this attribute to update, you have to double click on the Title Block and select "Reset Attributes".
         • 

     • DRAWN_DATE

       • The date the drawing was created.

     • DRAWN_BY

       • Pulls in your Autodesk profile information displayed in the upper right of the screen.

         • 

3. One huge disappointment when creating a Title Block within Fusion is the lack of drawing geometry accurately with dimensions as you draw.   Once you draw a line, rectangle, circle, or arc you can only go back and use the Inspect command (Inspect Panel) to measure what you drew.  You would then have to drag snap points to adjust the size.  Not sure why the same functionality you have in the sketch environment can't exist here so, as you draw you can place dimension to accurately layout and design the Title Block.  For example, if you use the rectangle command first there is no reference as to how big the rectangle actually is.  And you may end up drawing the rectangle that is 100 times the size it should be.  The line, circle, and arc command at least show a visual as to how big you are drawing.  So, if you choose this route to create your Title Block start with the line command so you have an idea how big you are actually drawing.

   • 

4. Modifying Title Blocks

   • To modify an existing Title Blocks simply select the Title Block and right click to choose "Edit Title Block".  Now you are back in the Title Block creation environment to make the desired modifications. 

     • 

Option 2 - AutoCAD

 

1. First things first, the AutoCAD file cannot contain any blocks information or Xref's so, you must purge the file of any of this information that may be hanging on in the background.  For more information of what's not supported click here.  If you have no idea what blocks, xrefs, purge or AutoCAD even is.  Sign up for one of our many classes on AutoCAD or stick with Option 1 above. 

2. Start at 0,0 and sketch in negative X and positive Y direction.  Below is a screen shot of Fusion so you can understand where AutoCAD and Fusion reference 0,0 from.  If you don’t start like this your Title Block will be off the border back in Fusion.

   • 

3. Borders can not be created independently like the Title Block but a custom Border can be included in a Title Block/Border combination.  Returning to Fusion 360 you would need to delete the existing Border if you go this route.  Also note that you can add things like proprietary notes, company information, standard notes… as well. 

4. Unless you have modified the standard Fusion border or are creating a combination AutoCAD Title Block/Border, it is good to know what dimensions you have to work with.  Below are the dimensions of all of the ASME and ISO borders to assure your new Title Block fits appropriately.

   • ASME Border Size (Actual X,Y) 
     • A 8.5in x 11 in

       • (7.74 x 10.50)

     • A 11 in x 8.5 in
       • (10.50 x  7.74)
     • B 17in x 11 in
       • (15.76 x 10.24)
     • C 22in x 17in
       • (21.00 x 15.50)
     •  D 34in x 22in
       • (32.00 x 21.00)
     •  E 44in x 34in
       • (43.00 x 32.00)

          

   • ISO Border Size (Actual X,Y)

     • A4 210mm x 297mm

       • (180mm x 277mm)

     • A4 297mm x 210mm

       • (277mm x 180mm)

     • A3 420mm x 297mm

       • (390mm x 277mm)

     • A2 594mm x 420mm

       • (564mm x 400mm)

     • A1 841 mm x 594mm

       • 811mm x 574mm)

     • AO 1189mm x 841mm

       • 1159mm x 821mm)

   • 

5. Attributes (AutoCAD ATTDEF Command) that translate over to Fusion properties must be named exactly as below.  No need to fill out the prompt or default option in the "Edit Attribute Definition" dialog box as Fusion will ignore them.   Any attributes you create that are named differently then what is below will come across as a custom attribute in Fusion.  How the attributes are mapped to Fusion properties were stated above in Option 1.

   • 
     
     • TITLE_1
     • SHEET
     • PROJECT
     • SIZE
     • SCALE
     • DRAWN_DATE
     • DRAWN_BY

6. Once you are finished laying out and designing your Title Block there is no need to block it in AutoCAD.  If you do, Fusion will fail to load it until you Explode the block and purge all traces of it from your file.  For me one thing I had to overcome is that Fusion is different than AutoCAD, AutoCAD Electrical, and Inventor and the information that I track in those programs doesn’t have to be included in my Fusion Template (but, can be).  Basically, I had to tell myself to Keep It Simple Stupid (KISS).  Below are some examples of simple and more complex Title Blocks.

   • 
   • 
     
     

7. Images in the Title Block

   • Even though it is mentioned above that Xref's are not allowed, an Xref'd Image is allowed.  If you have an image to place it can be placed through the Xref Manager (AutoCAD Xref Command).  These images will show once the Title Block is imported into Fusion.

   • Images can also be placed once you are back in Fusion by using the "Image" command on the Insert Panel.

     • 

8. Bringing the AutoCAD Title Block into Fusion.

   • Once the Title Block is finished save and keep this file in case changes are required.  If and when changes are required (Ever have a boss or customer change their mind?) this file can be modified and the changes can be brought back into Fusion. Follow the steps in the beginning of this article of how to add a Title Block from AutoCAD and re-select the AutoCAD file.  You will be presented with a dialog box to over write the existing one.

     • 
       

Conclusion

 

Whichever option you decide to create the Fusion Title Block.  I hope this finds you well, and sheds a little light on a few things.  And as always…..back to sweeping…..

Publish PDF from 2D CAD files - Synchronize the revisions and lifecycle of the drawing file and 2D PDF file

New for Vault Workgroup and Vault Professional 2020 is the ability to synchronize the lifecycle state (in addition to the revision) of the new pdf with the drawing file that created it.

In addition, PDFs can now be created at any lifecycle state in this release of Vault.  This is a big improvement from previous releases, where users could only create PDFs at the “Released” lifecycle state.

In this tech tip we’ll take a close look on how to set this up.

NOTE: The functionality described in this tech tip is dependent on the use of the Job Server and the Job Processor. This feature is available only in Autodesk Vault Workgroup and Vault Professional

Use Vault Workgroup or Vault Professional lifecycle states to trigger the production of pdf during a state change.

 

Configure PDF Publishing Options

Access the Files tab on the Vault Settings Dialog

Click Tools  Administration  Vault Settings.

Select the Files tab.

Select the settings for 2D AutoCAD and 2D Inventor PDF publishing.

Click Options... to configure PDF options.

The ‘Sync Lifecycle State and Revision As Source’ allows both the published PDF and its source file to have the same lifecycle state and a revision value.

PDF Category Assignment - Design Representation

All PDF files created for document control are automatically assigned to the Design Representation category. A dedicated category allows administrators to manage their rules, lifecycles, and properties independent of the associated design files.

This category has associated properties and behaviors that are applied to an object  when it is assigned to the category. Those behaviors are of three types:

• Lifecycles (files, folders, items, and custom objects)
• Revisions (files and items)
• User Defined Properties (files, folders, custom objects, and items)

Important:  To synchronize the lifecycle state and revision of the drawing file and 2D PDF file, set each file's Lifecycles and Revisions to be the same.

Engineering Drawings Category

            

Design Representation Category

Synchronized revisions and lifecycle of the drawing file and 2D PDF file

Revisions and lifecycle states of the published PDF are now synchronized with the revisions and lifecycle states of the drawing file.

Tip:  If your Drawing release process requires to change revision scheme - from Alpha to Numeric characters, for example – simply create a custom revision scheme (to be used for the Design Representation Category only) containing both Alpha and Numeric characters

For example:  A, B, C, D,…,Z,0,1,2,3,…99

The revision scheme assignment in both file categories will then be as follows:

Engineering Drawings Category

Design Representation Category

If the lifecycle of the 2D pdf file has not been set the same as the drawing file, the job processor will generate the following error:

Understanding Bill of Materials Structure in Inventor

Introduction

Throughout my time working as a design engineer the Bill of materials Structure always created issues for me and my colleagues. This is partly to do with the fact there are 5 types of structure and partly to do with every company operating by their own processes and procedures. I can’t help with the second issue but in this article, I hope to shed some light on the first to help you navigate to the right structures for you and your company.

The 5 BOM structures to choose from are:

• Normal
• Phantom
• Reference
• Purchased
• Inseparable

Understanding which of these structures to use in which situation can mean the difference between a complete Bill of Material and the workshop getting held up due to missing parts.

Accessing the Bill of Materials

First let’s see how to find the bill of materials! Inventor has a very nice dialog box that allows users to see and manipulate BOM’s from either the assembly environment or the drawing environment. In the assembly environment you can use the Bill of Materials command (see Figure 1) located in the Manage panel of the Assemble tab. In the drafting environment select either the drawing view or the parts list, right click and select Bill of Materials from the context menu.

Figure 1 - Bill of Materials command

When you enter the Bill of Material command you will be presented with a table like dialog box (See figure 2). In this table there are three tabs, Model Data, Structured, and Parts Only. The Bill of Materials table can be customized, and you can add and remove columns to suit your company requirements.

Figure 2 - Bill of Materials dialog box

Model Data shows all the components that are contained in the model and allows you to manipulate certain properties of the components from the top level assembly, a very useful tool when you need to manipulate the same property across many parts in an assembly.

Structured, as the name suggests, provides a structured view of the components in the assembly and displays it as it would be displayed in a drawing when placing a Parts List. This is an important distinction as the BOM structure of the components on the assembly comes into play here. More on this later.

Parts Only provides you a complete list of parts contained in the assembly. This can be especially handy for outputting a list of parts as it rolls up all common components irrespective of where they appear in the assembly structure. For example, you may have the same bolt that appears in both the top-level assembly and a lower-level sub assembly. The Parts Only would roll all these up to give you the total amount required of that bolt.

Bonus Tip: From the Bill of Materials dialog box you can export to Excel. With some filtering and the right BOM structure you can output a list of purchased components to send to you supply team!

Setting the Default BOM Structure

Setting the Default BOM Structure of a component can be done in two ways. Either through the BOM dialog box seen previously or using the Document Settings (see figure 3) when in the document you want to change. Once in the Document Setting dialog box navigate to the last tab (Bill of Materials). In this tab you can set the default BOM Structure (See Figure 4).

Figure 3 - Document Settings

Figure 4 - Bill of Materials Tab

Understanding BOM Structures

Now to the meat of the subject and how BOM Structure effects the parts list. Below is a breakdown of what each BOM structure is. It is important to note that these breakdowns are a high-level view and each structure type may have nuances not described here.

Normal:

This is the default BOM structure for part files and assembly files (excluding weldments). This means that a part/assembly will show up as a single line item in the BOM, the parts/assemblies will display normally in drawing views and the part/assembly will be considered in mass calculations.

Phantom:

This is a very handy BOM structure and has different effects depending on if the item is an assembly or a part. If you set a part to Phantom BOM Structure it simply will not show up in a BOM, however it remains a part of the assembly, displays in drawing views normally and will still be used in mass calculations.  If you set an assembly to Phantom BOM Structure it has a very different effect. It promotes the components in the assembly up one level in the Structured BOM (this promotion is signified by a blue arrow in the BOM dialog box, see Figure 5).

N.B If you have multiple occurrences of a phantom assembly the quantity of parts being promoted is multiplied by the quantity of the phantom assembly. E.g. if you have 3 bolts in a phantom assembly and 3 phantom assemblies the parts will show in the Structured BOM with a quantity of 9.

Figure 5 - BOM for a Phantom Assembly

Phantom Structures will also cascade. By this I mean components will continue to be promoted through the structured BOM until they encounter an assembly that does not have a Phantom Structure. An example of this is:

Assembly 0 is set to Normal and contains Assembly 1.
Assembly 1 is set to Phantom and contains Assembly 2.
Assembly 2 is also set to Phantom and contains Part 1.

The Structured BOM for Assembly 0 will show Part 1 as it will be promoted from Assembly 2 to Assembly 1 and then from Assembly 1 to Assembly 0.

Reference:

Other than Normal Structure most CAD users will understand Reference Structure. What this means is the part or assembly will not show up in a Parts List, will be detailed with dashed lines in drawing views (this can be changed in the view dialog box if required) and will not be considered during mass calculations. This is an important distinction between a Reference and a Phantom Structure.

 Now, there is another interesting nuance with the Reference Structure which is a component can be “set” as Reference by default or can be “overridden” as Reference in an assembly environment. To override the BOM Structure in an Assembly document you need to find it in the model browser, right click and select BOM Structure, and then select between Default and Reference. The difference between these two is often missed.

When a component is “overridden” as Reference it only appears as a reference in that particular assembly. Hence you can use manufactured components in drawing views (such as assembly documents) without it appearing in parts list or influencing the calculations but the manufactured part can be detailed normally in other assemblies or in its own context.

When a component is “set” as Reference by default it will always appear as a reference component in all the assemblies it is used in. If it is three levels down, it will still appear in the top-level drawing views as a reference file.

The difference between setting the default to reference and overriding the part in an assembly really is dependent on the component and the situation.

Purchased:

A purchased structure is just that. When you have a part or an assembly that is bought in you would set the default BOM Structure to Purchased. This essentially acts in the same way as a Normal BOM Structure where the item shows up in the Parts List, is displayed normally in drawing views and is considered in mass calculations with one major difference. When an assembly is set with a default BOM structure of Purchased none of the Children of that assembly will show up in the Parts Only list. The assembly will however show up in the Parts Only List as it is considered to be one part. See Figure 6.

Figure 6 - Purchased Parts

It is also very useful when exporting BOM’s to Excel as it allows you to sort between Purchased Parts and Fabricated Parts.

N.B. All content center parts are by default set to a Purchased Structure.

Inseparable:

Inseparable is the last BOM Structure available to you. This is the default setting for weldments but can be used for other situations as well. The Inseparable Structure is similar to the Normal Structure in that it appears as a single line item in a parts list, is displayed normally in drawing views and is considered during mass calculations. An Inseparable Structure will act as a Normal Structure when documented in its own context.

The Inseparable structure also shares a similarity to the Purchased Structure in that it appears as one line item in the Parts Only list. This is because it is considered as one part by the system despite it being fabricated with multiple components. An important difference between the Inseparable and Purchased Structure is that if you use a purchased part inside an Inseparable assembly it will show up in the Parts Only list as well. See Figure 7.

Figure 7 - Inseparable and Purchased

Conclusion

Understanding BOM Structure and how to set up your files can be complicated and will often require a lot of head scratching and multiple trial and error. However, once you have clarified where each structure should be used it can make BOMs much more complete and easier to manipulate, reduce errors in part ordering and improve company efficiency.