Monday, January 22, 2018

Surface Finish on Contoured Parts - Part 2

Milling the Fusion 360 Reciprocating Saw Demo

In part one of our blog on milled surface finishes, we looked at some generic information regarding surface finishes. In this particular blog, we will look at the steps used to mill a scaled-down version of the Autodesk Fusion 360 reciprocating saw demonstration and training part.

Note that this is just one of several methods that can be used to mill the part. Other people will have their own preferences with their own logic behind those preferences. Feel free to share your own tricks and experiences in the comments section.




Inspiration

The inspiration for this is the same part, milled full scale, by Titans of CNC to be used as a display piece by Autodesk at tradeshows. Titan's piece is fantastic, with a really good finish, but it also weighs about 60 pounds and is fairly difficult and expensive to ship to all the shows. (See Titan's YouTube video here)

Our goal was to mill a smaller version that could be used as a simpler and smaller showpiece. This was going to be milled on a Tormach PCNC 440, and was scaled down by half to fit into the work envelope of the PCNC 440. The question was whether we would be able to achieve a comparable surface finish to the Haas VF6 SS used by Titan.

Below is an image of Titan's part


Roughing

We utilized an Imco 3-Flute Streaker for the roughing. First a 1/2" diameter cutter (.52 DOC, .05WOC) to remove the bulk of the material, and a 1/4" diameter (.26 DOC, .04 WOC) for re-roughing or rest material roughing. 

Here is a slideshow, showing the roughing and re-roughing operations. Full video was difficult as coolant and chips obscured the video capture. 

When the 1/2" tool was finished it looked like the picture below. There is extra material leftover inside the pocket for the grip/handle, which needs to be removed by a smaller tool. Also, the stair steps are fairly large for the semi-finishing tools to be used, so it was our goal to smooth those out a little as well.

One can automatically re-rough the leftover material from previous operations. 
If you use a second adaptive clearing operation, depending on your parameters and tolerances, you may get some undesired air movements. John Saunders from NYCCNC did a really good video on removing the "whisper cuts", but those tactics do not always work on 3D contoured parts, plus we did want to knock down the stair steps a little.

Alternatively, you run the adaptive clearing just inside the pocket, so that the full material there is cleared away, then run some other cutterpath everywhere else. In this case, a contour cut. The two cutterpaths together allow for a smoothing of the rough model.
The roughed out part, from the 1/2" and 1/4 inch is shown below.

Semi-Finish and Finish

Although there are many different finishing strategies which can be used, we chose to use a combination of a parallel cutterpath (planar finishing), along with the contour cutterpath (Z-Level finishing) utilizing a slope option. For more information on the differences in strategies, and what the benefits of this are, see Part One of the blog.

This strategy was used for both the finish and semi-finish. Only the stock allowance and stepovers would differ. With Semi-finishing we left 0.005" of material for a finish cut with a .020 stepover. With finishing, we cut to net zero, with a 0.005" stepover. The two cutterpaths work together to cove the part completely, without large cusps or scallops remaining. 
After the semi-finish operation the part looked like below:

And during the actual finish process with the 3/8" ball



We used a 3/8" ball mill for most of the finishing, as it would deflect less than a 1/4 inch, and all of the radii of the part would still be milled. We used a 3/8" bull nose with a 0.015" corner radius for the bottom of the part to get a relatively sharp corner, yet still achieve a smooth finish.

Want to watch the semi-finish operation, check it out below. Sped up to save time.



Tips

During roughing operations, we had to pause four times to remove chips. Even so, many of the images during roughing show a lot of chips in the mill.

During finishing, we would check the runout in the tool and holder prior to milling. Using R20 collets, it is easy to have excessive runout if tightened too tight or put together incorrectly. We would check the runout and adjust the tool and holder until we could minimize runout, though we were never able to get it to zero. 

Polish

We can say the part is not hand-polished, but it is polished, so we can share another tip on surface finish. I have a friend that made small molds for the badges placed on cars. He would set several up on his mill at one time, program all of the parts, hit cycle start and practice some golf. Afterwards, he would place a small polishing bit in, with some compound, program that, let the machine run while practicing more golf.

In this case, you can use Dremel polishing bits with a 1/8" shaft. Simply place some polishing compound on your part, and use the polishing bit in your mill with a 3D cutterpath like Scallop. Let it go while you practice a round of golf, or do other work around the shop. For this part, we used the large cylindrical bit, approximately 0.42" in diameter and a spindle speed of 9000 RPM.


Conclusion

Milling 3D contoured parts is quite different from milling prismatic parts. Excellent surface finishes are possible, with almost all mills, with careful programming and strategies.








Friday, January 19, 2018

Surface Finish on Contoured Parts - Part 1

Surface Finish on 3D Contoured Parts

This blog is derived from a previous class at Autodesk University based on Surface Finish and can be found at this link

Special thanks to Imco Tools for providing the cutters for this experiment. Also to Tormach and their PCNC 440, where all the testing was completed. All cutterpaths were made in Autodesk Fusion 360

Surface finish is defined by:
  • Roughness - finely spaced surface irregularities. In engineering, this is usually meant by surface finish.
  • Waviness - measures of surface irregularities larger than roughness; usually from deflection, warping, or vibrations.
  • Measurement - Actual measurement of finish, either via contact or non-contact methods.
When dealing with 3D contoured parts, and parts used in moldmaking, casting, patterns, etc. we often use a "street" definition of surface finish, how much time will be spent polishing parts. As all CNC milled parts will have some form of tooling marks left on them.

When examining surface finish, you may often use some form of visual tool, such as the template shown below.

There are many factors that work together for your final surface finish, and some of those are:
  • Tolerances in CAM system
  • Toolpath styles
  • Stepovers
  • Tool types and holders used
  • Machine controllers and their capabilities
  • Rigidity and accuracy of the milling machine
This blog is going to focus on the CAM system; tolerances, stepovers, and toolpath styles.

This blog will use a relatively simple 3D Contoured part, which is actually a cover for a jack connection for a Fender guitar. If you would like the file to practice with yourself, you can download the STEP file


Tolerance or Chordal Deviation

When dealing with 3D contoured, you are dealing with faces. The cutterpaths created by the CAM system on the faces will be through many small straight line segments. These will be represented on your CNC mill as hundreds, and sometimes up to millions, of G01 point to point movements on your CNC machine. 

The chordal deviation is shown in the image below. The tighter the tolerance used, the more points that will be created during the CAM calculation.



On our part, you can clearly see the difference in the picture below. The only difference in the two parts is the one on the left was milled with a very loose tolerance of 0.12mm (.0047") and the one on the right used a tolerance of 0.01mm (.0004"). 


Stepover and Cusp heights

When finish milling 3D contour parts, ball nose or radius nose cutters are often used. When used, there will be scallops or cusps leftover from the are between the stepovers in the CAM cutterpaths. This scallop, plus a calculation are shown in the image below (R is tool radius, Cusp is desired cusp height, R-Cusp is used in the calculation)

Unfortunately, the scallop height calculation is only constant if the face is horizontal. When you have 3D contoured shapes and changing slopes, the scallop left behind actually changes, and often increases, as shown below, where the scallop on the right is actually higher than the one on the left, for the same stepover.

You can really see this come into play on the images below. Where the image on the left used a 0.8mm (0.031") stepover and the part on the right has a 0.254mm (.010") stepover. The difference in the roughness and cusp height is very noticeable



Cutterpath Styles

Good surface finishes for 3D contoured parts generally require tight tolerances and smaller stepovers. Also, the milling strategy can have a great affect on the finished part. 

Common cutterpaths for finishing include a parallel planes strategy (sometimes called parallel or planar), some type of top to bottom strategy (usually called z-level finishing, or contour or water level finishing), and a constant scallop options (sometimes called equidistant or 3D scallop finishing). 

Other strategies like morph and spiral are also available and may be covered in future articles. 

They all have their advantages and disadvantages, and you choose the strategy based on the needs and part geometry.

Parallel or Planar

This cutterpath strategy uses slices in the X, Y or some angle in between. 

Fast to calculate, this can leave larger cusps when steeper surfaces are more or less parallel to the cut direction as shown in the images below. The left is a parallel cut in the "Y" direction, and the arrow shows where the cusp may be undesirably high. On the right is the cut in the "X" direction, which has the same issue, just in a different location.


Z-Level Finish (or contour, or water level finishing)

Utilizing a Z_Level finish is very popular in moldmaking, especially with hard materials. The tool starts at the top and works it's way down, rather than going back and forth and "bumping" into walls and features. However, depending on the geometry shape, you still can have large cusps let behind as shown below.


3D Scallop (or equidistant)

Unlike the other two cutterpaths, this one does not utilize cutting by planes. The stepover is calculated in a 3D fashion, and the toolpath will keep making collapsing movements. This type of cutterpath will leave the same scallop or cusp everywhere, and usually have fewer retract movements in the process, all advantages.

One disadvantage of this type of cutterpath are tool deflections and vibrations are in different directions all the time, as the tool is sometimes going uphill than downhill than around, etc. Also, the collapsing corners can often leave finish marks on the part, sometimes affectionately referred to as "snail tracks". Shown in the images below.


Slope Based Machining

Planar cutterpaths work great on relatively shallow parts, and Z-Level cutterpaths work well on relatively steep parts. If you use the best of both of those on parts that have both shallow and steep parts, than you can get a great surface finish, and improved tool dynamics.

That is the concept of slope based machining. If 0 degrees is horizontal, and 90 degrees is vertical, then you can limit cutterpaths to certain sloped areas. The image on the left uses a parallel strategy, but only for an angle of 0 to 45 degrees. The image on the right uses a Z-Level strategy, for an angle of 40 to 90 degrees, allowing for some overlap. This completely finishes the part, and leaves no large scallops or cusps to be concerned with.

For the finished part using the combined strategy and slope angles see below:

Pencil Trace

Lastly as a tip, we would generally recommend running a Pencil Trace operation prior to your finishing operation. This will pre-relieve the extra material int he corners, allowing for a smoother finishing experience.

A pencil trace is where you run a tool in the corners of the part, at least the areas where the corner radius is about the same or smaller than the tool in question, shown below.


The difference in your finished part is fewer tool vibrations or getting "pulled in" the corners when finishing. In the image below, the part on the left did not use a pencil trace before finishing, and the part on the right did. Note the marks in the corners. Even though it was a parallel finish, the marks are normal to the surfaces, showing the tool deflected at those locations.


Conclusion

Use a tight tolerance and tight stepover for fine finishes, and match the cutterpath to your part, or use slope angles if appropriate.

Part 2

In the second part of this blog entry, we will look at how we milled the Autodesk Fusion 360 sample part, the reciprocating saw mold, on a Tormach PCNC 440, and got the desired finish as shown below.




Sunday, December 10, 2017

Jobs vs Research

30-second Challenge

Most people with milling machines are in the business of taking jobs and cutting them. However, once in a while, there is a question asked, or a challenge to be met, as is the case with our latest blog.

A company in particular, which we can not name, needs to face mill samples of material, which are then used for metallurgical testing. Depth of cut needs to be enough to get to get all the scale off and show clean metal. The question was; can this process be done on a small CNC, like the Tormach PCNC 440? Also, can the process be automated, and most importantly, can the cycle time be reduced to under 30 seconds?

In this case, tooling was provided by the tooling supplier, as well as two of the sample pieces. While the material is proprietary, we did learn the hardness was around 54-55 on the Rockwell C scale. 

The cutting tool supplied for the testing was a four-flute 1/2" dia cutter, with a 0.03" corner radius. Since we only had two samples available to us, we would not be able to perform dozens of speed/feed cut combinations.

We used HSM Advisor, with a downloaded power profile for the PCNC 440. After inputting some data, and doing some calculations, we were able to get the cycle time down to 23 seconds, as shown in the video below. You can hear the spindle draw as the cut starts, but it mills the pieces completely, and in 23% less time than requested.



Moving forward, the mill is large enough to hold several test samples. Either a custom fixture could be made, or they could simply use a self-centering vise, such as a 5th Axis Deuce, to hold multiple parts.

Other tooling to try

With this project, the tooling was provided. However, we would like to try inserted tooling to see if additional speed benefits could be obtained. Cutters like these toroidal cutters with round inserts may allow for additional chip thinning, and faster feed rates.

However, the project was definitely a success. We are able to get a more than acceptable cycle time, we can automate the process, and it can be done on an affordable, compact, CNC mill.






Thursday, November 30, 2017

Learn from my mistake, or why you should model your fixturing

Why you should include your fixturing in your model before CNC programming

I know, sometimes you're in a hurry, and you don't want to spend the time to import and model your vise, clamps, bolts, or other fixturing into your model before programming CNC cutterpaths.

But, how will you know whether your cutterpaths are completely safe without doing so? 

Well, we were in a hurry to start milling for our martial arts practice knife project. Even though we thought we had a high enough clearance plane set, turns out the washer made it just high enough to cause a problem. 

See in our video below:



Moral of the story is to include your fixturing into your model. 

Need to add basic components within Fusion 360? It easy to do, just use the included McMaster-Carr catalog, sort through the catalog to find your component, click the part number then the little "CAD" button. This will allow you to insert your component directly into your active model.



Save your tooling, don't let this happen to you.



Sunday, August 27, 2017

HD vs 2K monitor for CAD




When it comes to CAD, you want to use a monitor that is sharp, clear, and hopefully causes less eye strain. Resolution of the monitor has always been an important factor when in use for CAD. 

Once LCD flat screens became more commonplace and affordable, many people switched to using them. However, many early affordable flat screens were limited to a resolution of 1024x768. Many CAD users, with higher resolution screens, preferred and continued to use their high-resolution monitors, like the (very heavy) Sony shown below. 





With the introduction of HD (1920x1080) TV's and monitors, most CAD people switched to this format size. However, even an HD monitor does not have as high of a resolution as the old CRT Sony shown above, which was capable of 2304x1440 resolution.

Here at the CADCADZen labs we originally used dual 1920x1080 HD monitors for our desktop computer. These were used for surfing the web, office tasks and also CAD/CAM. We chose a 25" monitor over a 24" simply because the size difference is noticeable, where the 25" truly measures 25 inches diagonally, whereas most 24 inch monitors were 23.6 inches diagonally. 

In January of this year, one of the 25" monitors stopped working, and we needed to replace it. This opens up the possibility of going to a higher resolution monitor, such as a 2K or 4K, or simply staying with a cost effective HD monitor. 

Since we always have to consider the budget, I found a good deal on a 2K (2560x1440) monitor.  In this case it was the ACER G257HU. These can now be found online for around $200. 

To see the difference in resolution between an HD (1920x1080) monitor and 2K, see the image below.



On the left is a window of Fusion 360 limited to 1920x1080 resolution. You can clearly see from the background around it how much additional resolution (pixels) are available for display purposes. On the right is the same part loaded into Inventor utilizing the full resolution.

The purpose of today's blog is not to push a particular monitor, but rather to show you the difference between a 2K and HD display for CAD. However, this monitor is an IPS display, has good brightness, is quite sharp and had good reviews. 

The difference in CAD is noticeable. The sharpness of the part is better, CAM cutterpath display is improved, and overall use is more enjoyable. Some other advantages of switching from HD to 2K include:


  • YouTube videos played in a window are crisper.
  • Excel, Word and Outlook all display more data clearly. 
  • Work on more charts and graphs on one screen at one time.
  • Pictures from Digital SLR and Camera phones look sharper.

If you are looking at CAD monitors, and are still budget minded, consider a 2K monitor. In the long run we believe you will be happy you did. 

Maybe in a few years, 4K monitors will be priced lower, and we can do a similar story. Until then, we will continue to use our 2K screens for CAD/CAM, internet surfing and basic business work. 

About CADCAMZen:
it's the occassional thoughts, projects, musings, and opinions of a mechanical engineer that has been involved with CAD/CAM products for over 30 years.


Sunday, June 11, 2017

Creating a martial arts practice knife - Part 3

Training knife - Part 3


In parts one and two, we design the knife, fixture and manufacture the fixture. Here is how we milled the knife on the fixture.

There are many ways the knife could be milled, remembering we are going from a rectangular piece of material. You could step down with small steps as shown below. At times the tool will be at 100% width, but the step downs would be small.

Milling with step downs

Alternatively, you could mill sideways into the part as shown below. This does not work well because it wastes a lot of time in the air, and it runs into the neighboring knife.
milling with stepovers 


We could select just the geometry needed, and do an adaptive clearing as shown below. Then follow it up with a finish contour. This is the most efficient method, and safest.
Adaptive Clearing
Finish contour


To see the video, you can watch it below:





Sunday, May 7, 2017

Zen Tip 1: First thing to do in Fusion 360

First thing to do in Fusion 360:

You have Fusion 360 installed, what's the first thing you should do? Everybody will have their own opinion. One thing you could do first is set your Default Modeling Orientation

When you think of the TOP view of your model, do you normally associate that with the Z axis of your part or the Y axis? The default model orientation in Fusion is set so that Y is the normal direction for the top view. If you work in certain industries or do a lot of manufacturing, you may prefer to have the Z-axis be normal to the top view. 

Here is our video for our very first Fusion 360 tip.


Special thanks to GrabCAD, where I grabbed the model, and Scott Russell that put it there.

Top of the car corresponds to Z-Axis