Inventor HSM to DMS: 3+2 Axis Workflow

In this Instructable, I will lay out a detailed guide for how to take a complex 3-dimensional model from Inventor HSM and machine it using 3 axes, a part flip, and then 3+2 axes on the DMS router. This includes CAD to CAM, and CAM to machine workflow, as well as some general pointers that might help point out important things to notice along the way.

This Instructable is specifically catering to users of Inventor HSM and the Pier 9 DMS 5-axis router and Fagor controller, but most of the content will be generally applicable for users of similar software and machines.

Enjoy!

Step 1: Create Your Solid Model

First, you'll need a model. Create the geometries you need in Inventor, or import them from another program - just make sure they're solid!

The model I'll be using was captured with Autodesk's free software 123D Catch. There is an Instructable here on how to bring that into Inventor.

Step 2: Create Stock Material

Once you have your model created, you have to prepare it for HSM, or CAM software.

This means you'll have to choose what stock material you need to start with in order to contain your part all inside the material you choose. Additionally, you have to make sure you have somewhere to hold your material while leaving enough room for the cutter to machine your part without damaging the vise or clamps!

I will use a vise to start on the first side of my stock, before flipping it over and using strap clamps to hold it down to scrap board to machine the opposite face. So I made stock material that encloses my part entirely with at least 0.1" to spare on all sides. The square bottom shape allows for the vise to grab securely, and the flanges on the top face will make it easy to hold the material down with strap clamps (photos in later steps).

The stock can just be extruded over the entire model, and then features to be machined can be pulled over them in the project tree. You can see the spherical extrusion is reintroduced to the stock material.

Step 3: Prepare Your Model for HSM

Add a UCS - a user- or work-coordinate system in a logical position that you can reference in the machine. This will allow you to tell the machine exactly where your part sits in physical space inside the machine, relative to its home position. Popular choices are corners or centers of edges and faces. Mine is in the upper near left corner.

If your part (line mine) is going to require a flip or repositioning, make sure you make a reference mark on your piece that you can use to create a new UCS for the second side. By using the machine to actually create the new position, you can be sure that you're registering the other side of your part perfectly to the coordinates the machine was using for the first operations - errors aren't carried forward. This also requires that you align perfectly straight stock well to the bed of the machine - a vise is a great way to do this...

Note: if your stock isn't perfectly square, use the machine to cut a parallel notch that you can use to align your work with the direction of travel when it is repositioned! I didn't do this because I was using squared stock in a well-aligned vice.

Step 4: Use HSM to Create a Setup for Your Machining

Now that your model is prepped for CAM, it's time to use HSM to get the toolpaths going for the machine.

First, you need to tell HSM what you want it to work with. This requires imagining how the machine will remove material, and ensuring that you are properly representing where this material is! Otherwise, you'll end up crashing into the material unexpectedly, or cutting air for hours...

So, first you create a setup and select the UCS you created as your coordinate system - "Select coordinate system" in the pull-down menu. Then select your model.

Then in the next tab, you might want to double check that the dimensions on your bounding box of stock material in yellow match the material that is in your hands. Check the rounding factor. Obviously, cheating the machine to think there is extra material will be safer - because it will cut air that it thinks is your part. But the reverse can be really bad, especially with hardwoods or metal! Just check that everything matches.

Step 5: Create Your First Operation

I'll start with a lot of detail about the first operation, and just add specifics for later operations...

First, select an appropriate tool for your first operation - for me this will be the reference for my part flip, and I'll use a medium sized tool so the radius doesn't obliterate the flat faces I need to measure against later. Use the largest tool you can, in general. The work will go faster.

Check that the speeds and feeds look right based on your experience with the tools and materials... If you have none, seek counsel! You can also check FSWizard for a good starting point, although there speeds tend to be on the aggressive side. I'd recommend taking off 40% to start. Don't assume the speeds and feeds are correct! They are often automatically very fast or slow!

Then, select the contours that you want to machine in the Geometry tab. I selected the top edge of the spherical exstrusion - imagine the material seen from the top, and your defining the outer limit. You can adjust this by picking if its an outside, inside, or center bound, and offset it by any amount.

In Heights, I used a lower bound to make sure that the tool would not go low enough to run into the vise, but would go entirely through the bottom of the flange.

Under Passes, pick a conservative maximum stepdown. If you're not sure, starting at 10% of tool diameter is a fairly safe start. Adjust as you learn the materials! Optimal load will likely be set to just under the radius of the tool, which is ideal. In this case, a fine step down is specified, which means the center will be cleared with the max stepdown, and the surface will receive a finer treatment with smaller stepdowns.

Step 6: Clear the Bulk of the Material Away From Your Part

I start machining by using an aggressive and intelligent strategy called Adaptive Clearing to remove the most material I can before adding a fine polish to the part with more delicate operations.

Using an Adaptive, I first selected the tool (same warnings always apply!) then the geometries constraining the limits of what I want it to touch. Without a proper boundary, the tool will pass all over every edge of the part all the way to the bottom - a sure way to hit your workholding devices.But since a boundary is selected, it will just go to the bottom of that feature, so the Heights can remain unchanged - top to bottom.

I set slightly more aggressive Passes depths at 20% of my tool diameter. In wood with a 1" tool, I could probably even double this number. Start conservative and work your way up!

Step 7: Surface Your Part

There are many different surfacing strategies that all use different methods of small stepovers to create a smooth surface. This is normally done with a ball end mill, since it doesn't have any sharp corners that will leave deep marks in the surface. I'm going to use the biggest ball end possible, to leave the smoothest scallop I can, since the radius of the sphere is much larger than that of the tool. If you want to capture fine details, a smaller ball end mill is needed.

I'm going to show how to use Contour (a vertical stepover) and Scallop (a horizontal stepover) together to match the way the sphere transitions from steep at the edges (vertical) to shallow in the center (horizontal).

First, I created a scallop with a ball end mill on my sphere geometry, then I set the height to go down to a point just below what felt like the inflection point of steep to shallow. This is just a rough guess by eye. But note, I set the lower limit to 2.5" from model bottom. This will be important in a second.

Then I created a gentle 0.020" stepover - a relatively small increment compared to my 1.000" tool. Each pass is 0.020" lower. You can see a preview of this toolpath.

For the Scallop, I adjusted the top boundary to be just above the previous bottom boundary, to help blend the two toolpaths together. The top starts at 2.7" from model bottom, 0.2" from the previous low mark reached by the Contour. Note, these heights always apply to position of the very bottom of the tool, not the tangent point where it touches the material.

Make sure the stepover on the Scallop matches the Contour!

Step 8: Simulate!

Now watch the simulation to make sure it looks like you expect! Watch carefully.

You can also check the total time of your setup, to see how long it will take in the machine. This estimate is usually pretty reliable, but will take longer if you have to stop frequently to make sure everything is going according to plan.

Step 9: Post-Process

Once you're satisfied, use Post Process.

For all you Pier 9 users: select just one operation at a time!

Post Process using the post script titled DMS fagor 8055i M5xS_R5.cps that can be found on the Network drive in the folder called CNC Data, and add that to your Documents > Autodesk > Inventor HSM 2015 > Posts folder, and restart Inventor HSM. The generic DMS Post creates problems on our DMS Fagor setup! Dan the Man has made this Post specially for us. Use it! Thank him!

All files should have the naming structure xxxxxx.pim, where x's are 0-9 numerals. I titeled mine 000101. Adding a comment can help you remember which code name was which operation. I added "Reference Machining."

Step 10: The First Set of Operations - in Action!

Breaking up the how-to's with a few photos, that hopefully help connect the toolpath with a visual of how it actually looks in real life!

Important things to notice: how rough the rough pass leaves the material, and how the thinner, lighter, Contour leaves a fine dust and a smooth surface. This not only is the best way to get clean parts, but also the fastest!

Note: not pictured was using a spot drill to pin-point the exact upper near left corner of my workpiece just as it is pinned as the UCS in the model. Make sure your part is oriented correctly in X and Y before you start!

Step 11: Redraw Your Model for the Next Step

Here, you can see I've redrawn the boundaries of my stock to expose more complex features that I'd like to machine before I flip the part over. This could have been integrated into the first section as well.

I exposed the features I want to machine, then added tabs to ensure that my part remains connected to the flanges that will be held down after the flip. By adding them into my model, I am guaranteeing that the machine won't ever cut my part completely loose. Mine are about 1" wide by 0.75" tall, which is maybe a little conservative, but prevents chatter that can create a rough finish.

Then I extruded a cylinder into the spherical area I have already machined, in order to protect it from subsequent operations. This will prevent the machine from trying to work in that area, which would mostly be wasted time cutting air. This can also be achieved within one setup by using the "Rest Machining" check box.

I saved a new version of this file, so I could be very specific with these different configurations. Again, this all could have been done in one setup and one model, depending on what's easiest for you.

Step 12: Use HSM to Prepare Toolpaths

Moving a little more quickly now...

I created a new setup using the same model and UCS, and then did an Adaptive Clear with a large, flat end mill, then repeated the Adaptive with Rest Machining and a smaller 1/4" tool. This way I could get into the nooks and crannies in preparation for surfacing, which was also going to do with a 1/4" tool, except for the Contour I switched to a ball end mill for a smooth surface.

Note that I did not take these operations all the way to the bottom of the model, since after the flip I would be able to reach some of the deeper areas (and undercuts!) much more easily. The Adaptives go just a bit deeper than the Contour.

Step 13: More Action Shots

Here are those last steps in action.

Notice how the surface is somewhat spotted in the last photo - the tolerance/smoothing for tight curves can be set in the Passes tab, and can tuned to create even smoother surfaces, sometimes at the expense of machining time. I planned to sand everything later, so this was plenty smooth for my purposes.

Step 14: Cut Fixture Material (optional)

Now, I was ready to flip my part over and work on the other side. However, because of the complex geometry, most or all of my part is floating off the surface of the table, so it would likely vibrate and machine poorly if it wasn't better supported.

In order to reduce chatter as I worked on the other side of the hands, I chose to machine a styrofoam filler for the sphere inside the hands. Because the shape was very easy to match and model, it was an easy choice to include the extra support. I used an Adaptive and a Contour, and then cut it off on the bandsaw.

Step 15: Fixture Material for 3+2 Axis Machining

When it is time to flip your part for 3+2 axis work, it is really important you properly secure your material, but also leave room for the head of the machine to get right up close to your work piece, and for the cutter to not run into your clamps.

You can see I'm using styrofoam and double sided tape to create a larger area of contact between the workpiece and the table, but also that all the supporting material is softer than the work material, in case the tool runs into it - this way I don't need to model the styrofoam or worry too much about it.

Once it is firmly secured to a scrap board to prevent accidental machining of the table, I used flat metal pieces to ensure that my piece was well aligned with the axis of the machine, using the slot cut for the vise, which is perfectly in the X-direction.

After that, I used strap clamps on three of the sides to firmly secure the workpiece, while leaving the fourth corner with the reference notch open. Using the edgefinder, I was able to locate that corner of my workpiece, which allowed me to tell the machine exactly where to start from on this side. As you'll see, this 0-0-0 position corresponds to the UCS I set on the next version of the model I used.

Once this origin was set in the machine, I clamped down the final strap clamp. All of them are as far away from the working area as I could move them.

Step 16: Prepare the Second Side of Your Model

Once you're all set to go on the other side of your part, similar preparations need to be made as earlier on...

I have modified the stock extrusion to leave the hands completely exposed now, but left a little artificial surface below the palms, which will act as a bounding box for the Adaptive Clearing I'll use to remove the large amount of material around the hands, without cutting the air above the flanges where there is no material.

Then, I have added cut-outs to allow clearance for the tool and spindle to work around the edges of the model. As you'll see later, I ended up cutting even more material away to make even more room for the head of the spindle.

Finally, I assigned a UCS on the now-top-surface of the reference I machined at the very beginning. This needed a couple other notches just to allow me to point X and Y axes in the correct directions when prompted, but I won't actually machine those pockets in the actual material - they are just for my reference in the model.

Step 17: Work From the Top

Now that my work is fixtured and my model is re-oriented, I'm ready to use HSM to prepare the toolpaths for the flipped side of work.

The Setup involves creating a stock material that includes the flanges and the unmachined material around the hands, as well as the air above the flanges. The UCS over the machined area is assigned as well. Be sure your flip in the real world matches your flip in the model! You can see the old UCS as a reference.

In order to not spend time cutting the air above the flanges, I've specified in my Adaptive operation to just cut above the profile outlined in blue, which is why I left that surface in my model. You can see the operation only works on the center of the part, which happens to correspond to where there is material. The adaptive then does rough clearing of the material around the hands.

Then a Contour is used to clean up the surface, but as you can see in the last photo, I did not send it all the way to the bottom, since I was going to use 3+2 axis machining to come at this complex geometry from the sides.

Step 18: Machine the Top Down Operations

Check out how the HSM toolpaths look in real life.

Step 19: Prepare the Model for 3+2 Machining

The major change in 3+2 axis machining is defining a new axis within your operations for the machine to view your model from. This means creating plans referencing origin places or existing surfaces in your model. In my case, all the new planes are at 45 degree angles to horizontal, just to give a better angle on some of the detailed parts of the model.

This also requires you to carefully draw bounding sketches around the areas you would like machined. Since now the Z-axis is measured perpendicular to the new plane, not the table of the machine, you have to specifiy a tight area in which you'd like to have the tool make cuts. You can see in the photo how I sketched on one of my 45 degree reference planes the area in which I wanted machining to occur.

Do this for every angle you'd like to machine from.

Step 20: Use HSM to Prepare Your 3+2 Operations

The same setup could be used for the 3+2 operations as was used for the previous vertical milling operations.

Start by clearing out the bulk of the material between the strap clamps in order to give the head as much clearance as possible.

Step 21: Contour From All Four Sides Using 3+2

Now it's time to machine from a new angle.

First, start a contour like normal, straight from the top. Under the geometries tab, click the "Tool Orientation" box, and select the reference plane for that side of 3+2 machining. Use the model to select directions for the coordinate system, and don't forget to select a bounding box from the sketch drawn on that plane, to tell the tool where to stop.

Check out the model from the side, and see how deep the Z-axis should go under Heights. I made sure mine cleared the finger tips, and didn't go too far up the top side of the hand, since that was already machined from the top.

Then look at the toolpaths from the "top" (reference plane POV) and side, so make sure things look OK.

Repeat this process for all sides of 3+2 machining.

Step 22: Simulate!

Do a check, like always, to see that the tool is behaving how you'd expect! The simulation works fine from the new axis - it just might do some funny things to your stock material simulation, if you check the box "stock." Use common sense to identify where you still have any stock material left - probably not much left anywhere!

Step 23: Finally, 3+2 Axis Machining

Another chance to quickly see how those choices in HSM played out for me in my final part.

At this point, I was ready for cutting off the tabs, and finishing the model by hand.

Step 24: Digital Becomes Physical

The satisfaction of finally getting my hands on the wood after all that time on the computer and at the machine is always so gratifying.

It would be possible and a great fixturing exercise to machine away the tabs. In metal, this is usually a great idea, but in wood, it comes away so easily under hand tools, the tabs are easy to shape to the curves in the model using chisels, gouges, rasps, and sandpaper.

Many hours of fixturing and HSM time spent holding and shaping the piece in my own hands for about an hour. The call is up to you.

Good luck!