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Fusion 360 - Center Line Hack

Here is a hack for adding a center line to a detail view. Before we get going if Fusion 360 had a "Break View" (Create a foreshortened view with a section of the part removed) command I would have used that instead. But, here we are.

When you have a design that is long, sometimes showing its entirety in a drawing view leads to dimensions going to features that are hard to make out when printed.

This is exactly what I ran into. I wanted to have the middle of my design "blown up" on the drawing so the end user could tell exactly what edges the dimensions are going to. In my case, I wanted to identify and dimension off the center of the part.  Since, there is no "Break View" command the only thing I could do was to use the "Detail View" command and show the middle of the design.  Here lies the problem. The "Center Line" command requires picking two edges to identify where the center line is placed. The newly created "Detail View" isn't showing the two ends to create a center line.

Fusion offers the ability to sketch on top of the view but, it is very limiting and there is no good way of locating the "center line" accurately. Even if you could locate the line it can produce incorrect dimensions depending how the are placed. If you click on the sketch geometry first it pulls a dimension from the "Sheet" and likewise, if you click on the parts edge first it pulls a dimension referencing the model. Not to mention that the dimensions seem to always go in as "Disassociated Annotations" and you can never be re-associated.

The only viable solution for me was to create a sketch in the model and name it "Center Line" then turn on the visibility in the view. Note, the line cannot be a construction line because it will not show in the drawing view. The line must be a "normal" line. The added benefit here is the sketch and drawing dimensions are parametrically linked so when the design changes the drawing will update accordingly.

Autodesk is currently planning on a "Break View" command but, it appears to be something in the future.  You can read it for yourself here.  

Hope this finds you well and helps out in some way! Time to go sweep!

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…..

Autodesk University 2019 - IMAGINiT Manufacturing Instructor Sessions Now Online for free

That's a wrap on Autodesk University 2019. This year at AU, 15 of our Autodesk-certified instructors shared their product and industry knowledge with the thousands of professionals in attendance. 

Didn't make it out to AU2019? No problem! View on-demand recordings of our IMAGINiT Manufacturing and PLM instructor's classes, download handouts, view slide decks, and more. 

Manufacturing and PLM Presentations:

• Rusty Belcher, Solutions Consultant
      Process Modeling Essentials for Industry 4
  
  
• Anthony Dull, Solutions Consultant
      Vault for the Revit User
   
• Caleb Funk, Solutions Team Manager
      Sharing Is Caring: Sharing Vault Data Outside the Firewall
  
  
• Pete Markovic, Senior Solutions Consultant
      Mastering the Fusion Lifecycle App Store in 60 Minutes
   
• Robert Savage, Instructor
      How to Use Fusion 360 and Inventor for Effective Designs
      Fusion 360 Introduction to Generative Design
   
• Stan Wile, Application Engineer
      Supplementing Your Designs with Inventor CAM and Inventor Nesting 

Generative Design with Fusion 360

Introduction to Generative Design with Fusion 360

 

Want to learn more? Take this and other manufacturing courses from IMAGINiT instructors at Autodesk University 2019!

 

Overview of Generative Design

Generative Design mimics nature’s evolutionary approach to design. Designers or engineers input design goals into generative software, along with parameters such as materials, manufacturing methods, and cost constraints. Unlike topology optimization, the software explores all the possible permutations of a solution, quickly generating design alternatives. It tests and learns from each iteration to ascertain what works and what doesn’t. Generative Product Design breaks down into four components: the function of the part, materials used, the manufacturing process, and how it needs to perform.

The function of the part is a combination of loads and forces that are applied and known physical constraints that restrict the space and mounting points. In traditional design methods, you take the information you know and mix that with traditional shapes to develop a couple of concepts then you run an analysis on each iteration to look for the best performance. With generative design, you build bodies that represent preserved areas, obstacles, and starting shapes. You will apply loads and constraints to these bodies to help define the function of the part.

The material that is used for the part design can vary and has a direct effect on the strength of the part. In a traditional design setting, the material is not necessarily known until the part is created. You start with a single material, then adjust based on the outcome of the analysis. With generative design, you assign multiple materials so that you can optimize your design process.

The manufacturing process of the part is also not always known and can range from machined, cast, fabricated or printed. With traditional design, the manufacturing process is typically determined by the design of the part. With generative design, you select from a list of options to derive results based on the options selected.

At this point, you begin comparing the results to decide what is the best option to use. Traditional design requires that you review the part design, the part analysis, and the manufacturing options to decide which design fits your specific needs. Generative design allows you to compare these options all in one place, then simply download the desired solution that best fits your needs.

 

The Process

This is an example of a common design process used to develop and evaluate a design chosen to be run through a Generative Design software. 

1. Identify the problem domain and gather information: Spend some time thinking about the problem at hand and how it fits into the greater context of your operation. Ask yourself: How does the new part(s) interact with the greater assembly? What kind of manufacturing, assembly, or other practical considerations is present? Are there any dynamics at play (e.g. moving parts, changing loads, etc.,)? What is my end goal - is it weight/material reduction, performance enhancement, aesthetics, or some other metric improvement?

2. Create preserve geometry: Start with the existing base model, be it a single part or a full assembly. Create the interface geometry (e.g. bolt bosses, flanges, etc.,) as new bodies to be used by the generative process. Be sure to include any needed extra grind/machine stock, fluid containment walls, or other "oddball" preserves.

3. Create obstacle geometry: Again, working with the base model, create any obstacle geometry needed. This might include fasteners (nuts, bolts, screws, pins, etc.,). It also might include more complicated geometry like swept solids (e.g. the path a toggle clamp makes as it swings into position). Be sure to include any needed tool clearances (wrench or ratchet). One "gotcha" to keep in mind: people often create obstacles that are too short - make sure your obstacles clear the envelope of the problem setup.

4. Set up your boundary conditions: Specify the constraints, loads, manufacturing details, and materials into the system. Be sure to build your load cases based on any dynamic motions that may be involved (for example, a part of a car suspension may experience braking, acceleration, turning, or stasis).

5. Run your studies: At this point, run your various studies. Pay attention to early results to ensure that you're getting the expected kinds of solutions. You'll notice fairly early on if an obstacle is too short or if you've forgotten some specific detail.

6. Examine your results:As your results are delivered, use the tools available to determine which solutions are worth further investigation. This may be a combination of using scatter plots, visually comparing possible solution results, or inspecting the model stress visualizations.

7. Compare results to initial expectations: Circle back to step one and validate what results were generated against what you expected or desired. You may discover that a result didn't quite make it to the end and needs to be pushed through as a starting shape to further refine it. Maybe you have an intriguing result that would make a great starting shape for a secondary study. Perhaps you've identified some results that you would like to validate with an additional FEA package.

8. Integrate back into the base: Once you've generated a result that you're satisfied with, export it as a BRep/TSpline and place it back into the base model to inspect the context again. Begin thinking about next steps with regards to CAM, 3D printing, CAE validation, etc. Add in required features like machining operations or modify the TSpline as needed to achieve your contextual requirements.

9. Take next steps: Take your final model out to CAM, CAE, 3D printing software, or whatever the next stage is for your design.

10. Rinse and repeat: Continue working through this process iteratively to further refine your designs.

 

Fusion 360’s Generative Design is utilized in many areas of design - from Architecture through Manufacturing. If you would like more information on Generative Design and will be attending Autodesk University this November 2019, we recommend these courses: 

TR323048-L - Fusion 360 Introduction to Generative Design

MFG331809-L - Generative Design Boot Camp for Product Design and Manufacturing

MFG323797 - How to Use Fusion 360 and Inventor for Effective Designs

 

I would like to thank Kenny Cornett for his input and feedback on the content of this document.

 

AutoCAD to Fusion 360 Sheetmetal

Often times I run across a client that wants to convert their 2d sheet metal flat patterns into 3d models. These flat patterns are trusted and has been successfully manufactured year after year.  Using Fusion 360 the designs could simply be recreate and flattened.  But, the odds of getting the new Fusion 360 flat pattern to lay exactly on top of the trusted flat pattern would be a difficult and time consuming task. 

The Fusion 360 Team has now added a "bend" command to sheet metal which allows us to successfully tackle the task described above and have faith that when we flatten the design it will lay exactly on top of our original flat pattern. So, moving forward the Fusion 360 file would become the official document of record.  Where we can take full advantage of everything that 3d has to offer.  

Before we jump into Fusion 360 lets first take a look at what the file looks like in AutoCAD. Make sure that the bend lines are not set to a continuous line type.

 

If the lines are set to a continuous line type then when we go to select the object in Fusion 360 incorrect areas will get selected.  Also, please make sure that all of the actual edges of the sheet metal are on the same layer so, that when the profile is selected it recognizes all of the internal cutouts.  If the internal cutouts are on layer "A" and the outside profile is on layer "B" the internal areas will not be detected.  And would add more time in the converting the design to 3d because you would need to manually select the internal cut areas.  Like the image below.

Now that we have some house cleaning out of the way let's get started.  How do we get the 2d into Fusion 360?

 

If you are using Fusion Team which I hope you are.  Then I would copy and paste the 2d files directly into your drive and the files will just show up in your Data Panel.

 

I will assume for now that you are not using Fusion Team and just want to get the file into Fusion and start working.  Create a new sketch and go to Insert DXF.  Select your DXF and choose what layers to bring in and make sure that the Insert Mode is set to "One Sketch per Layer" then hit OK.

 

Select the Flange command, choose the sketch and select the appropriate sheet metal rule and hit OK.  When using the Bend command it is crucial that you work from the outside of the part to the center of the part.  If you think about it, it just makes sense.  If I started in the center of the part and bent the part up 90 degrees the sketch with the bend line is still laying flat.  So, I wouldn’t be able to continue bending the part because the part is now up in the air and the bend lines are still on the original plane.  There will be times, that no matter how careful you are you may need to create a new sketch on the part and draw in a new bend line.  I will show you an example of that here soon. 

Select the Bend command and choose the area of the sheet metal that you do not want to bent and then select the bend line.

Continue working from the outside to the center of the part. 

Here is an example of when you still may need to create a new sketch and a new bend line.  In the below image Fusion 360 will not allow me to bend the wings up 90 degrees because the model will self-intersect. 

 

So, the body of the plane needs to be bent first.

 

The only problem is the part bends and the sketch that we inserted stays on the sketch plane.  So to finish the wing a new sketch needs to be created on the part with a new bend line drawn in. 

So, experiment with this workflow and I will get back to sweeping some mines. 

Hope this helps you in some way!

 

P.S

Depending on how you bring in the 2d data the history may be turned off in your design and you may not see any sheet metal functionality.  Simply right click on your timeline and select "Capture Design History".

Creating Conical Sheet Metal Components in Autodesk Fusion 360

Autodesk Fusion 360 does not have a specific command that will allow the creation of conical sheet metal components, but with a little creativity, the process is easy!

The first step is to create a constrained sketch of the desired conical component wall.  I have used a base radius and an angle, or you could use the a top radius instead.

The next step is to use the Flange tool to turn the sketch into a sheet metal component.  Selecting the conical side sketch, set the distance to a very small value.  In my example, I am using -0.001 in because I would like the flange to be on the outside of my sketch line.  Select the desired sheet metal rule and select OK to finish. 

Below is a close-up view showing the sheet metal flange and the sketch line at the top edge.

At this point note the model parameter assigned to the sheet metal thickness (rename for easy recall).  Select the “Change Parameters” command on the Solid > Modify tool panel and expand the sheet metal parameter for the sheet “Thickness”.  In my example it is “d4”.  I have made it a Favorite for easy to access.

Next, make sure that you have made the original sketch of the conical component visible so it can be used in the next step.  Change the Fusion 360 environment to either “Patch” or “Surface” depending on which user interface you are using (I am using the new UI Preview user interface).

Using the Revolve (surface) command, select the visible sketch and either the vertical construction line or the origin axis as the revolve rotational axis, and rotate to create a surface body of the required number of degrees.  IT IS VERY IMPORTANT not to rotate a full 360 degrees so a gap will be available in the conical sheet metal body to unfold it later.

The last step in the process is to use the Thicken command in either the Surface or Solid environment to thicken the previously revolved surface body to the same value as the sheet metal flange created earlier using the parameter value I just made a Favorite. Two important things to remember are:

1. Make sure the thickness is a negative value, so it is created on the same side of the surface as the sheet metal flange created earlier and
2. To make sure the “Operation” is set to “Join”. What this does is make the thickness become a part of the sheet metal flange thus making the entire conical body a sheet metal component.

All done!  Now you may select the Create Flat Pattern command in the Sheet Metal environment, select the inside surface of the conical sheet metal component as the Stationary Face and finish by picking OK.

Using variations on this modeling technique, you can create truncated conical sheet metal components with intersections such as the one below.  The one thing to remember is to do all body cutting to the surface body BEFORE using the Thicken command.  This will give you clean square edges to your flat pattern layouts.