Check out a Tips and Tricks session using CAM for Fusion 360! Curt Chan, our CAM…
Turning Point – New Turning Updates in Fusion 360
Check out What’s New in Fusion 360 Turning
NEW! – This post has been updated with improvements and features from the January 2019 release. They are marked as New but organized into their respective sections below.
The Fusion 360 CAM team has been busy improving turning in Fusion 360. Keqing includes these updates in the big What’s New blog posts, but there has been so much goodness added recently I thought it was worth calling out all of the turning updates and enhancements. We’ll take a deeper look at some of the updates made since September, and why and how they can improve your turning process. The improvements are listed below and grouped together based on the part of the toolpath they impact. A big thank you to Akash Kamoolkar and Angelo Juras on gathering all this information below!
When defining a custom tool holder for either a General Tool or Boring Bar, the Leading Angle and Trailing Angle parameters can be defined for the holder. These parameters ensure accurate results, especially when visualizing the tool holder during creation and stock simulation. I’m sure I don’t have to elaborate on why accurate stock simulation is important!
Setup – Parametric Safe Z
The first thing to note here is the renaming of the “Home Position” Setup parameter to “Safe Z.” You’ll find this parameter when creating a new Setup after choosing Turning/Mill-Turn as the type. This change helps clarify the difference between the Safe Z and the machine home position at G28 or G53. Safe Z refers to the position the tool retracts to between machining operations to avoid interferences or collisions.
Now on to the meat of the update. The Safe Z can now reference the Stock Front or Back in addition to the WCS Origin. This gives flexibility to users who might want to place the WCS Origin somewhere like the back of the stock, but reference the Safe Z from the front of the stock. This should make it much easier to ensure adequate clearance between operations – less math and large offsets. Just select the Reference and input an offset where a positive value will move the Safe Z in the Z+ direction and a negative value will move the Safe Z in the Z- direction.
Cutting Below Center
There was always a single face pass included in the Profile finishing operation, but it only brought the radius of the tool tangent to the centerline, leaving a little nub or cone on the end of the part.
This update pushes the initial facing pass down so that the tool goes past the centerline by one corner radius, removing the extra material left on the end of the part. This eliminates the need for hand finishing or additional operations just to get rid of that little nub. For extra control over how far the tool can go past the centerline, there’s a new “Distance to Cut Below Inner Radius” parameter in the Radii tab. This parameter allows you to cut past the Inner Radius to help remove any small nubs on the part. Enter a positive value and the tool will go that distance past the center. This is available in Profile and Grooving.
NEW – Facing During Groove Goes Below Center
Similar to the improvement above, Grooving finishing operations were not facing down to the center when there was an axial hole. They would just face down to the hole, leaving the center of the part un-machined. This left an unfinished face on the front of the part or required an additional finishing pass to finish the entire front face. Now the initial facing pass in the Groove finish operation will go down to the center, as shown below.
We also added the “Distance to Cut Below Inner Radius” parameter to the Groove toolpath to allow the grooving tool to go a certain distance below the inner radius, as mentioned in the update above. This parameter allows you to cut past the Inner Radius to help remove any nubs left on the part. This distance is in addition to the tool nose radius.
NEW – Profile Corner Control
You can now control the shape of the profile turning toolpath at outer corners using the parameter “Make Sharp Corners” in the Passes Tab. This checkbox is unchecked by default, meaning the outer corners of the toolpath are smoothed with arcs. When this parameter is checked, outer corners in the toolpath are machined without arcs. Sharp corners can help with toolpath readability, and may look more familiar if you’re used to hand programming turning operations. Basically, you want your toolpath to look how you want it to look, and we want to help you get the toolpath you want. Note that the resulting part will not be changed – this parameter only affects the toolpath corners.
Approach and Retract Z
The Linking Tab of every turning operation now has an “Approach & Retract” section where you can set the Z position of the tool before and after the operation. The options are the Safe Z or the First/Last Toolpath Point. The exception is Internal Threading where the Approach and Retract Z will always match the Safe Z position to reduce the chances of a crash.
Override Safe Z
When you select Safe Z as the Approach or Retract, you can also use the “Override Setup Safe Z” checkbox to override the Safe Z defined in the Setup. This gives even more control over the Safe Z at the operation level. For example, one operation might use a tool that’s especially long and requires a larger Z retract to safely clear unfinished material.
Fixed Lead Directions
“Use Fixed Lead Direction” is new to the Linking Tab of Profile and Groove operations. This checkbox determines how the Lead Angle affects the Lead-In/Out moves. Checking the box means the Lead-In/Out moves are relative to the Z-axis of the Setup WCS. When the box is unchecked, the Lead-In/Out moves are relative to the toolpath.
Pull Away Before Retract
The Pull Away Before Retract parameter overrides the Lead-Out Angle to avoid collisions with the stock. Checking the box may result in slightly different Lead-In/Out moves than specified, but leaving the box unchecked can result in stock collision. We recommend checking this box for safer lead angle results.
Fusion 360 checks every lead to see if there are gouges with the solid model or the remaining stock. This helps make sure the toolpath is will run safely. If a gouge is found, the “Lead Mode” alters the Lead-In/Out as follows:
- Fail – Toolpath generation will fail if it’s not possible to create the linking moves without causing a gouge. You will need to make adjustments to make the lead-in/out moves fit and generate.
- Discard Passes – Discards any passes that cannot be reached with the current linking settings. This would create rest material for the next operations.
- Move Lead – Moves the lead to a different location along the part until there is room to execute the lead as specified.
- Turn Lead – Changes the Lead Angle parameter until there is room for the lead as specified in the other parameters.
- Retract Lead – This is most automatic option, which is why we recommend it for the easiest way to get safe results. It will adjust the linking parameters so all links are safe and acheivable, and in some cases will use a Radial Retract when there are no other options. This is also the default setting.
When making finishing passes for Profiling and Grooving operations, we suggest making a separate finishing operation using Rest Machining. This helps ensure the operation calculates with the proper rest material. That means gouges are identified more accurately and can make the resulting Lead-In/Out moves more predictable.
We are excited about the many recent updates to Fusion 360’s turning functionality! I’m looking forward to sharing even more of the team’s hard work in the future. Keep an eye out for the new update in January for even more turning goodness. In the meantime, we want to hear from you! Ask any and all of your Fusion 360 CAM questions on the CAM Forum. Let us know your ideas for future improvements on the Fusion IdeaStation.