Autodesk 360 – CAM

Titans of CNC

If you want a much better explanation of how to machine this part, check out Titans of CNC video lesson series. Titan put together truly amazing classes and the one of the best features of the Titan courses are they are all free. 

You will learn how program parts in a way that they are machined in the real world.  The advice and skills freely given thought the series is real enough to get you a real job. 

But, why the extra blog post. Well, I needed to make my own notes so I can adapt what Titan shows us how to do, in a way that will run on my tiny SainSmart toy CNC.

I think the SainSmart machines are close to being a good learning tool. They are a bit too small and need some actual clearance to make any real part. But, I think it’s an easy fix. I even see some ways of doing it myself. But I am hoping SainSmart beats me to it. 

If you are from SainSmart and reading this. Please note, I work as an Independent Contractor and I would be happy to help.

New Setup

Once you have a part drawn. Navigate to the Manufacture tab of Autodesk 360 in the upper left hand corner. Start a new setup. In this step you will select:

  1. The milling operation
  2. The model orientation
    1. Select z axis/plane && X axis
  3. The stock size

Set Origin (X - Y - Z zero)

A common place to put your x-y-z zero is the upper left hand corner of the part. This is because that side of the jaw does not move (generally). 

Do this by selecting Select z axis/plane && X axis. 

Select the top face for z and a line along the x axis for x. Flip the axis as needed.

Set-Origin x-y-z Autodesk 360

Set Stock Size

Pick – Add stock to all sides. This allows you to pick how much stock is on each side of your part. 

Programming Tool Paths

Titans machines are way more powerful than the SainSmart. But I will show the tools he uses and the speeds and feeds. It is going to be higher than what we can do on the SainSmart. 

Setting Tool RPM and SFM

Your machine will have constraints as to how fast the spindle rotates (RPM) and how many surface feet per minute it can translate (SFM). 

These two equations can be helpful in setting the feeds and speeds of your machine. 

CNC Feeds and Speeds

 The Harvey Performance Company has a good article explaining the subject of feeds and speeds. It is worth a careful read. 

For more reading and charts see Machinery’s Handbook. For engineering guidelines see Marks’ Standard Handbook

2D Face - Operation

You will need to ‘deck’ off the top of the part with a face mill. At a maker space you might have a 1 insert 3 inch fly cutter. You will want to run this around 800 RPM on a a standard Bridgeport machine. On a modern CNC machine with modern tooling, even a low HP machine, the settings will be higher. 

Face Operation - Tool Settings

First you will set the tool perimeters. This is shown as the first icon in the top menu if the facing operation in Autodesk Fusion 360. 

Feedrates are set to 4000 rpm and 25 in/min because that is what a typical modern low horse power CNC machine can handle. Your machine is probably different. You will need to program feeds and speeds that are suitable for your machine. 

Face Operation - Geometry Tab

Set each ‘from’ to ‘model top‘. This is an easy way to think about where the offsets should be set. But remember you need to have enough clearance between the model top and whatever fixturing you have. Model top is Titan’s standard, I will go with that. 

Face Operation - Bottom Height

Autodesk 360 confusingly calls the depth of cut the bottom height. Whatever you set your bottom height to is the depth that your cut will be. For this facing operation you want the bottom height to be 0.00 in.

When you are programming other operations, such as 3D adaptive clearing, you will set the bottom height to the depth of cut. 

Face Operation - Passes Tab

As we move along the top tabs of this operation we get to the passes section. Remember you can read each of the descriptions and get to know what each setting does. 

The pass extension is the distance the tool will travel once it has disengaged from the part (after cutting) This is somthing you want to set for a facing operation, otherwise the surface finish of the part will be different on one end of the part. 

Set this to to more than half of the dimeter of the tool. Said in another way, you want the center of the tool to be off the part by more than the radius. 

Face Operation - Pass Extension

The pass extension is the distance the tool will travel once it has disengaged from the part (after cutting) This is somthing you want to set for a facing operation, otherwise the surface finish of the part will be different on one end of the part. 

Set this to to more than half of the dimeter of the tool. Said in another way, you want the center of the tool to be off the part by more than the radius. 

A Note About Stepover

Stepover does not need to be set in this case, but in other cases this is an important setting. Stepover is the amount the tool will move over (or stepover) after each cut. This means how much the tool will step over into the material to be cut. If you set the stepover to a large number, the machine will have to work harder to clear the material. So be careful with this setting and understand it is an important setting. 

Roughing The Outside of The Part and Pockets

You can use 3D adaptive clearing to rough the outside of the part and the pockets

3D Adaptive - Tool, Speeds and Feeds

The tool chosen in this case is a 3/8 flat end mill.

The photo below shows how to set the speeds and feeds. As before we are at:

  • 4000 RPM
  • 25 in/min For Cutting Feedrate, Lead-in & Lead-Out 
  • 15 in/min For plunge and ramp
  • Surface Speed will be calculated by Fusion 360
This is the first feature I am cutting with the SainSmart. I dont have a fly cutter for it, nor would I advise trying…

 

Here are the  feeds and speeds for my SainSmart.

  • 1/8 in wood router bit
  • RPM 3000
  • 10 in/min For Cutting Feedrate, Lead-in & Lead-Out 
  • 5 in/min For plunge and ramp

3D Adaptive - Geometry Tab

A brief explanation of some of the setting in the 3D adaptive clearing.

3D Adaptive - Machining Boundary

Set to None so the program knows to cut all stock that is available. Said another way, it will cut without bounds. 

3D Adaptive - Stock Contours

Again you want to select Nothing so it mills everything possible. 

3D Adaptive - Rest Machining

This is an important setting because it tells the program that it does not need to re-cut anything that was cut in a previous operation. With Rest Machining selected, it will know what material was already cut in a previous operation, so it does not need to go over that section again. Instead it will move right over what still needs to be cut and start right where it needs to.  

3D Adaptive Clearing - Heights Tab, Autodesk Fusion 360

3D Adaptive - Heights Tab

Again set all to Model Top. When you set the bottom height to -0.76 in. you are telling the machine to face the outside of the part down to -0.76 in. The two pockets will be selected next and that selection will tell the program to machine down to the bottom of the pockets. 

3D Adaptive - Passes Tab

Optimal Load is an important setting. This can be considered the Stepover. Said another way this is the amount the program will try to take off the part during each pass. Since we have a 3/8″ tool selected and we are going all the way to the bottom of this part, we will set this to 0.100″

Minimum Cutting Radius is increased to give the tool more room on inside corners of the part.

Maximum Roughing Stepdown is set to 0.80 in this case. Since the tool will healical into the part we want to go all the way to the bottom of the pockets and we want to rough the outside of the part in one shot.

Stock To Leave should be set to 0.01 on the bottom (Radial) and the sides (Axial).

3D Adaptive - Linking Tab

Set the Stay-Down Level to 70% this will allow the tool to lift up and go over the part after it finishes roughing the outside. If it was set to most, the machine would stay down and move all the way around the perimeter of the part. 

Lift height could be set to bring the tool up slightly in-between cuts. In this case it can be left at 0.00 because it is slightly faster.

No-Engagement Feedrate controls how fast the machine moves when it is not engaged with the part. 100 in/min is pretty fast for smaller machines. The SainSmart can only do about 30 in/min max.

Horizontal & Vertical Lead in/out radius is the radius the machine takes as it moves to engage with the part. 0.150′ is what we have here. 

Ramping Angle is the angle the helix will be at as the tool enters the part. For a smaller machine you will want a smaller ramping angle. 1 degree is acceptable. 4 degrees will be more aggressive. 

Helical Ramp Diameter: The tool here is 3/8′ or 0.375″ the Helical Ramp Diameter should be a bit smaller than your tool. That will cause the toll to overlap as it helicals down. 0.350″ is good here.

Minimum Ramp Diameter: You can put 0.3 here.  

3D Adaptive - Simulate The Toolpath

Be sure to select show stock. You can make the stock transparent so you can see the part inside the stock as it is being cut. Having the stock opaque has its advantages also. 

Create The Finishing Passes

We will use the same 3/8″ flat end mill as before and take off the last 0.100″ that we left on the part during the roughing passes. The feeds and speeds should automatically be filled in the same way you set them in your the 3D Adaptive clearing. 

2D Contour - Geometry

Select the bottom contour (or tangent chain) of the part. 

Geometry Tab - 2D Contour Fusion 360

2D Contour - Heights Tab

Be sure to select model top for each section again. Be sure to set the depth of the cut to 0.76″ again. These settings are the same as the heights tab for the 3D Adaptive Clearing above.

2D Contour - Passes Tab

Choose climb cutting, for compensation type set wear. This will allow the machine operator to adjust the compensation, if needed. Of course, my SainSmart does not have this feature. 

 

Passes Tab - 2D Contour

2D Contour - Linking Tab

Most of the default values here are good. You can change the Lead-In Sweep angle to 45 degrees. This has a more gradual lead in to the part. 

Linear Lead-in distance can be increased to give the tool room to lead in. 0.100″ is a good distance here. 

Vertical Lead-in Radius is not needed here and can be set to 0.00″

Entry-Points: This is where you select where the tool comes down to the part. The default location for tool entry is at the origin, in this case that is the back of the part. It is preferable to have the entry point at the front of the part so you can see the tool come down. 

For Entry-Point, select the front right vertical corner of the part and the tool will come down there. 

Finish The Pockets

Use 2D Pocket for this. We will be using the same tool and the same feeds and speeds as the 2D contour, so those should be pre-loaded into this toolpath. Let’s move on to the geometry tab. 

2D Pocket - Geometry Tab

Select the pockets. They will turn blue

Geometry Tab - 2D Pocket Fusion 360

2D Pocket - Heights Tab

Select model top for everything here again. Set the bottom height to 0.5″ because that is the depth of our pockets.

Heights Tab - 2D Pocket Fusion 360

2D Pocket - Passes Tab

Since this is a finishing pass with some contours, bring the Tolerance and the Smoothing Deviation down to 0.0004″ 

Set Maximum Stepover. Here is is 0.25″ This is a finishing pass so it is not as critical here. 

Unclick Stock to Leave because this is a finishing pass. 

 

2D Pocket - Linking Tab

Un-click Keep Tool Down it is not needed here. Change Lead-In Sweep Angle to 45 degrees as before. For ramp we can select Plunge because the material is already milled out. Ramp clearance height.

Linking Tab 2D Pocket Fusion 360

Chamfer Edges and Locate Holes

We will use a 1/4″ chamfer mill and the 2D Chamfer toolpath. You will need to set your speeds and feeds for this tool. You can use the same values as before. 

Geometry Tab

Select the top most line for the chamfers, especially if the chamfer is modeled into your part. 

 

Geometry Tab 2D Chamfer Fusion 360

Heights Tab

Set everything to Model Top as before. For the bottom height enter 0.00″ The tool will compute the offset.

Heights Tab - 2D Chamfer Fusion 360

Passes Tab

Set Tolerance to 0.0004″ and Compensation Type to Wear. Set Chamfer Width to 0.01″ This is the actual width of the Chamfer you want on the part after the machine makes its pass. 

Chamfer Offset can be set to 0.050″. This means the chamfer mill will both move over 0.050″ and drop down 0.050″. 

Chamfer Clearance can be set to 0.0″ here because the chamfer mill can move all around this part without colliding with the part. 

Linking Tab

Horizontal Lead-in Radius 0.025″ and Lead-in Sweep Angle set to 45 degrees as before. 

Duplicate Toolpath for Lower Chamfer

The lower chamfer is pretty much the same as the chamfer above. You will need to:

  • select the new geometry
  • Set bottom height to -0.5 inches
  • And be sure to set your Chamfer Clearance to 0.050″ Autodesk will know to keep the tool 0.050″ away from the part.

Spot Drill Holes

Select the drill toolpath. We will slow down our feed rate to 10 in/min because we are actually feeding the tool into the part. Select a face of one of the holes then click on Select Same Diameter to automatically select the other holes. 

Geometry - Drill Toolpath Fusion 360

Heights Tab - Setting the Chamfer Diameter

Set all to Model Top as before and use the same settings as above. The Bottom Height this will actually be setting the Chamfer Diameter. But what should we set that to? Here it is. 

The tool is 45 degrees so this is a 90 degree included angle. If we drop the tool 0.050″ the diameter of the hole we make will be twice that depth. So it will be a 0.100″ diameter hole. 

We have a 10-32 bolt going in this hole. The Major diameter of a 10-32 bolt is 0.190″. Let’s add a 10% chamfer on the outside of this hole. So, the chamfer diameter will be 0.190″ * 1.1 = 0.209″. Divide this number by 2 and you get 0.1045″. 

Set the bottom height to 0.105″ 

For the cycle tab, you can leave it to Drilling – Rapid Out.

 

Heights Tab

Program The Drill

We will use a 0.1772″ Solid Carbide 2 flute Drill. Choose Drill Toolpath. Select Tool. Feed in at 15 in/min. Retract Rate can be 40 in/min.

Select the same faces of the holes as you did in the previous step.

The drill needs to be deeper than the tapped hole because there is a section of the tap called a lead in. The tap lead in can be measured with a comparator. Or kinda guess with a calipers if that will get you a good enough tolerance. In the threads need to be 0.380 deep. We are going to go 0.200″ deeper for a bottom height of -0.580″

Cycle Tab

We will choose Deep Drilling – full retract for the Cycle type. This will peck and retract all the way out of the hole each time. Breaking off the chip and allowing coolant to get into the hole. 

Pecking Depth can be set to 0.050″ and Minimum Pecking Depth can also be set to 0.050″. 

Drill Cycle Type

Tap The Holes

Select the Tap Toolpath. For the tool we will use a #10-32 Roll Tap. Set spindle speed to 1000 RPM. Or slower on a smaller machine. Be sure you are above the minimum speed on your machine otherwise the plunge rate and spindle speed will not match. 

In the heights tab set all to Model Top, as usual and set the bottom height to -0.480.

For cycle choose Right Hand Tapping. 

Right Tap

Simulate The Entire Part

Right click on your setup. Choose simulate and you can watch your entire part be cut. 

Simulate Part - Fusion 360

Reorder Your Tools

If you look at the toolpath tree, you will see that the tools are out of order. You will want them in the correct order when you load this program into your machine. So go to the upper right hand corner of Fusion 360 and select Manage and Tool Library. In the tool library manager click the 1-2-3 button in the upper right hand corner of that screen. Leave all to defaults and click OK. This re-orders your tools for you. 

You want to make sure your hight offsets and diameter offsets match perfectly. 

Reorder Tools - Fusion 360

Post Process Your Part

This is where you actually generate the G-Code for your machine. Go to the top ribbon of the Manufacture tab in Fusion 360. Look in the Actions section and click on Post Process.

 

Your Done!

I highly recommend checking out Titan’s course. You will learn a ton if you can stick with it. Be sure that you run these parts on a machine. Otherwise it will be hard to know what you really did. 

You will need to update the speeds and feeds for YOUR machine. 

Leave a Comment

Your email address will not be published.