Advanced Routing MDF

1

So I wanted to share a case study that I am working on with MDF cutting

Here are the details

Material: .22" MDF Eucalyptus based (not pine fiber mdf)
Tool: Onsrud 57-266 3/16" 2-flute downcut wood rout
Recommended Chip Load for x1 Dia: .006-.008"

Non-Changable Parameters:
Tool Diameter 3/16"
MDF Material
.22" DOC
Downcut tools only

Machine Used :
CNCRP PRO4896
2.2KW GMT Air Cooled Spindle 8000-24000rpm
No Vacuum Table
MDF Spoilboard only

Material Attachment Method:
18ga pin nails down each side of the sheet in the y-axis direction

Part Details:
Monogram Names varies (lettering)

Part Holding strategy:
Triangular tabs used .3" width and .055" height at programmers description

Objective of Case study:
Increase Tool Life
Minimize breakage of thin Script fonts
Improve cycle time
Minimize Chatter

So I have been working on this for awhile and want to share some recent discoverys that some people might not be aware of. That being that MDF will produce a “chip” when cutting if your using the proper tools

Why do we want “chip formation” when cutting really any material? Because its all about tool life and minimizing heat build up at the tool. If you are running your tools properly you will save money on expensive carbide

I am running a relatively low horsepower machine and spindle and not the most rigid set-up compared to more industrial like production machine. So I am very rarely able to achieve the proper chipload for a given tool. Some work-arounds are running your spindle at lower speeds but that requires more spindle horsepower so that might not always be the best option. Another option is to reduce your depth of cut and take more passes but this can cause a substantial increase in cycle times.

So we must look elsewhere for solutions to our problems and one possible solution will reside in the the proper tool selection for you application

We have a couple options on tools to evaluate

  1. 2-flute downcut wood rout
  2. 2-flute downcut chipbreaker
  3. 1-flute o-flute downcut spiral
  4. 1-flute compression spiral

2-Flute Downcut Wood Rout tool:
This tool has been my go to tool for quite some time now but I find that I am only able to get between 5-8 sheets life span. This is due to the fact that I am not able to run this tool at the proper chipload but I can get close as you will see in the picture on how we start to see chip formation and not dust

2-Flute Downcut Chipbreaker
These tools are great for low horsepower machines but I decided against this due for a number of reasons including material, part geometry, surface finish, cycle time, tool change

1-Flute O-Flute Downcut spiral
These tools are a great option for low horsepower machine because of how the tool geometry cuts into the machine. Also single flute tools are capable of achieving a higher chipload at a slower feedrate. These tools are commonly used in hard plastic cutting but will produce a superior surface finish in composite woods

1-Flute Compression Spiral
With the benefits of the above tool this tool has one disadvantage on thin .22" mdf and that is the length of the upcut section and the tendency for it to lift the material from the spoilboard due to our work holding strategy. Now I am experimenting with a 3/8" diameter in 1" thick mdf next as I will be able to get a mortise compression tool and achieve the proper chipload on my low horse power machine

So now that we have evaluated some tool options lets see some results with specifically the 2-Flute Downcut Wood Rout

Photo 1
Is showing the typical dust that is formed when typically cutting mdf without the proper tool chipload. This will introduce excessive heat into the tool and shorten tool life. Although the dust created does help with part holding

Here where my settings on these chips:
18000rpm
150ipm
.22" DOC
130ipm 3 degree linear ramp
.0042" chipload

20180408_092749
20180408_0927492851Ă—2138 2.01 MB

Photo 2
Is showing that we are starting to get actual chip formation from the mdf material. This is good that means that we are getting closer to removing that heat and preserving tool life. Also we get the added advantage of shortening cycle time. However there are 2 disadvantages 1 being decrease part holding and minor increase in chatter due to the thin material

Here where my settings on these chips:

16200rpm
220ipm
.22" DOC
160ipm 3 degree linear ramp
.0069" chipload

20180408_092736
20180408_0927362851Ă—2138 1.62 MB

Photo 3
Is showing that chips are not getting compacted in the cut path when running the tools at a higher chipload there are almost completely evacuate via dust collection

20180408_092902
20180408_0929022851Ă—2138 1.8 MB

Just thought I would share my findings here let me know if you have any questions

2 Likes
3

thanks :slight_smile:

5

@BillBlades

oh yeah man sure shoot me the link !

7

nice!! thanks

9

Good work on this Evann @WorkinWoods . Clearly you spent a lot of time on your case study.

If I may ask, respectively, would you please edit the title of this post to something a bit more appropriate? Perhaps something like “Advanced Routing Speeds into MDF”. I am not disputing your case study content but I do think its a bit misleading and a little too much for new “XCarve” owners to be introduced to such high speeds. Might I also suggest that you put the post into the “upgrade” category or something of that nature…

Easel has requirements set for MDF with a 3/16" bit at 40 ipm and a DOC of .0625" for a reason. Is that too slow? meh, perhaps… but it also allows people to get better acquainted to the feel of their machine and its capabilities before jumping into warp speed. Reading your post suggests that its ok to ramp up to those speeds out of the gate… which we all know is not the case.

To be clear, I am not looking for a p*ssing match… just think its not a fair comparison when comparing your 8’x4’ CNC to an XCarve machine.

and honestly… I almost crap my pants when my Xcarve goes up to 100ipm at .03"DOC using a 1/4" bit… I cannot imagine running it at the speeds you suggest and that deep… :slight_smile:

Ron

1 Like
10

yup I will change the title and I put it in the un-catagorized area because I didn’t know where to put it move it to the category of your liking

and really I am just explaining concepts on how to properly run tools and with anything on the net its up to user discretion and its more just to get people thinking how researching machining techniques will benefit there business

11

I hear ya… and again, not disputing the content. Nor do I think anyone will…

I personally think its amazing what some can do with their machines… but just because the odometer on my SUV says it can go 240kms doesn’t mean I should . :slight_smile:

Might be cool in your case study to also show the chip differences between 40, 60, 80 and 100ipm… both deeper and more shallow DOC. just a thought…

Happy carvin…

R

(EDIT. Thanks for changing the title…)

1 Like