Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

How can I define an HEM toolpath when I cannot override both the cutting feedrate and the FPT?

12 REPLIES 12
SOLVED
Reply
Message 1 of 13
simspacetn
428 Views, 12 Replies

How can I define an HEM toolpath when I cannot override both the cutting feedrate and the FPT?

In Fusion 360 CAM I'm trying to define high-efficiency machining (HEM) toolpaths for a 5/8" end mill where the ADOC is 2x the tool diameter and the RDOC is 20% tool engagement. When I apply all the correct tool parameters in my feeds & speeds calculator, the adjusted cutting feed rate (IPM) for chip thinning is 111. And the adjusted chip load (FPT) for chip thinning is .0052".

 

When configuring the tools cutting data in the tool library, I can set the ADOC and RDOC with the values I mentioned above. However, when I change the FPT to .0052" it automatically calculates the IPM as 91.37". And when I change the IPM to 111" the FPT changes to .0063". It appears I can only change one or the other, but not both.

 

The Fusion 360 formula for chip load is tool_FeedCutting / (tool_SpindleSpeed * tool_NumberOfFlutes). It does not appear to take into account a a radial chip thinning factor (RCFT).

 

My feeds & speeds calculator uses the same formula, but it does includes a radial chip thinning factor (RCFT) that is calculated as follows: (CuttingFeed / (SpindleSpeed * NumberOfFlutes))*RCFT

 

Where RCFT is:

simspacetn_0-1690062239944.png

 

Am I misunderstanding something about how Fusion 360 and HEM toolpaths work? Maybe I don't fully comprehend how 2D and 3D adaptive toolpaths work and what's going on under the covers? I thought they are related to, or are an implementation of high-efficiency machining (HEM).

Thanks!

Chris

Labels (1)
12 REPLIES 12
Message 2 of 13
a.laasW8M6T
in reply to: simspacetn

There's some funny business going on with your calculation

 

Fusion does calculate the feed rate correctly given the correct parameters

Because you haven't stated what rpm you are going is suspect possibly you have a different number of flutes defined in fusion than you do in your F&S calc.

 

or you F&S calc is giving you incorrect info, because table feed(in/min) ALWAYS equals rpm x feed per tooth x number of teeth

 

To answer your question about adaptive toolpaths, yes they are designed to take advantage of HEM and radial chip thinning, but Fusion doesn't need to account for the Radial chip thinning etc, that is what you F&S calc is for.

 

I think you are misunderstanding how the RCTF formula applies, it would normally be used in the case where a manufacturers f&s chart has a feedrate specified for 50%+ engagement(where the chip thickness is highest).

 

If you were using 20% engagement you would use the formula to figure out what the new feed per tooth and table feed are, they will increase according to the formula, but what stays the same is the CHIP thickness.

 

 

Feel free to ask more questions too i'm not super great at explaining this stuff.

also any extra info you can supply can help

like which f&s calc, which tool and coating, which material etc.

Message 3 of 13
brad.francola
in reply to: simspacetn

Hi.  Are you sure you have the correct number of cutting edges defined for your tool?

Message 4 of 13
simspacetn
in reply to: a.laasW8M6T

Maybe a good place to start is for me to share my feeds & speeds calculator I created. It's a Google Sheet:

https://docs.google.com/spreadsheets/d/1ueQnyYNvrOG-4vOUOuDwcEHpGPhn0EejuZGqypUAjVs/edit?usp=sharing

 

I created the calculator to do a deep-dive into learning about speeds, feeds, chip thinning, HSM etc,. Fill in the orange(ish) fields in the far left column and the spreadsheet formulas do the rest. You can also override RPM in cell B12.

This is one of the main sources I used during my feeds, speeds and HSM toolpaths discovery:
https://www.dapra.com/articles/radial-chip-thinning

For a quick background, I'm fairly new to CNC machining. I got my first VMC last August. I'm fairly competent in Fusion 360, but still learning tons. I'm still a little foggy on the adaptive toolpath details. I use them all the time but I'm still foggy on their relationship to HSM and what's happening under the covers, which I know is a lot.

Thanks for the replies @a.laasW8M6T and @brad.francola!

Message 5 of 13
simspacetn
in reply to: brad.francola

I do have the correct cutting edge count. It's a 5 flute 5/8" flat end mill.
You can see that info in the feed and speed. Calculator, I attached to my previous post.

And I checked my design and the flute count is correct in the tool library.

Thanks!

Message 6 of 13
simspacetn
in reply to: a.laasW8M6T

@a.laasW8M6T 

 


also any extra info you can supply can help

like which f&s calc, which tool and coating, which material etc.


I am cutting 1"x1" 1018. I'm using this Hass HSPM2 series of end mills which are which is TiAlN coated.

I provided a link to my S&F calculator in a previous which is a Google sheet.

 

 

To answer your question about adaptive toolpaths, yes they are designed to take advantage of HEM and radial chip thinning, but Fusion doesn't need to account for the Radial chip thinning etc, that is what you F&S calc is for.
....
If you were using 20% engagement you would use the formula to figure out what the new feed per tooth and table feed are, they will increase according to the formula, but what stays the same is the CHIP thickness.

 


I think this is my primary area of confusion with F360. I use the formula to figure out the FPT and IPM, but in F360 they are not mutually exclusive,  if I change one the other is updates automatically. I can't set them independently of each other to match the calculator results.

 

But maybe that's where the adaptive toolpaths come in? I supply the RDOC (20% engagement) and either the chip load or the table feed from the calculator, and the adaptive toolpath compensates for the appropriate chip thinning at the higher feed rate? I don't know, This is where I struggle understanding adaptive toolpaths and what they are doing.

 

Also, I wouldn't be surprised if I am using RCTF incorrectly. I was drinking through a firehose when I was trying to absorb all I could on feeds, speeds, HSM, chip thinning, etc.

 

I trust F360, but I would love to have a better understanding of how HSM and chip thinning are implemented in the app in relation to the data I am entering.

 

Thanks,

Chris

Message 7 of 13
a.laasW8M6T
in reply to: simspacetn

I can't see your spreadsheet, but have requested access.

 

"This is my primary area of confusion with F360. I use the formula to figure out the FPT and IPM, but in F360 they are not mutually exclusive, that is, if I change one the other is updates automatically. I can't set them independently to match the formula results."

 

The thing is, they CANNOT be independent, hence me saying there must be something funny going on with your calculation, if we can get to the bottom of that i'm sure it will be clear.

 

Its great you are doing a deep dive and using a spreadsheet etc as its a good way to really understand what is going on.

The .pdf you linked is a very good description of chip thinning, I would suggest re-reading it to try and understand what it's telling you(For me I go through an iterative process of reading resources, applying what I think I understand, seeing if it makes sense, reading again and so on until I am pretty sure I have a good grasp of the concepts involved and how to apply them)

 

Now another thing is that for HEM, RCTF is only one part of the reason HEM works well, there is another component that is more difficult to explain.

 

Applying radial chip thinning !=HEM

you also need to factor in heat generation and what that allows you to do to your surface speed.

generally the less  RDOC you use the more you can increase your SFM(and therefore RPM), which for a given fpt means more ipm.
What the optimum Rdoc is depends on your ADOC and the material.

More Adoc=less RDOC, harder material = less RDOC

So optimum for mild steel may be 20%, toolsteel could be as low as 4-5%, and aluminium 30% or more.

See these screenshots for the FSWizard app I use:

First has chip thinning turned on but HSM turned off:

Screenshot_20230723-122433.png

Second has HSM turned on:

Screenshot_20230723-122449.png

 

You can see the SFM increases which give more IPM even though the FPT is the same.

 

You can also see the HP usage goes up so you need to consider that your machine has enough HP to take the cut too.

(for example I use a 12mm endmill in mild steel at 10krpm and it uses all the HP my machine has)

 

 

Message 8 of 13
simspacetn
in reply to: simspacetn

@a.laasW8M6T, I gave you editor permission.

 

I do use the free version of FSWizard. I need to try out the chip thinning and HSM options.

 

I agree with your iterative reading process comment. I do that a lot. It's super helpful and reveals things I missed in the first and second passes. In fact I'm about to re-read your post again. 😁 

 

Thanks! 

Message 9 of 13
a.laasW8M6T
in reply to: simspacetn

Your adjusted IPM formula should simply be number of teeth*rpm*adjusted FPT:

formula.png

 

I think you were applying the chip thinning factor twice? which was how you were getting the erroneous result

Message 10 of 13
simspacetn
in reply to: a.laasW8M6T

Oh wow .... good find. Thank you @a.laasW8M6T 

Message 11 of 13
seth.madore
in reply to: simspacetn

@a.laasW8M6T wow, you dug into this topic pretty deep!

 

I have a bit of "caveman" approach to speeds and feeds, especially in the more "forgiving" materials (I don't do this for exotics)....Manufacturer recommendations, reduce by 20% or so, observe and listen to the cut. If it's off a theoretical small percentage from ideal, I really don't sweat it 🤣


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 12 of 13
a.laasW8M6T
in reply to: simspacetn

Yea, I mean what the F&S calcs give you doesn't always work, so you have to try it out and see how it runs on your machine/setup.

 

I machine a lot of stainless and have settled on feeds and speeds that have been adjusted till i get it to run nice and get decent tool life, it all comes from experience really.

 

For Aluminium, I'm at 150% of the manufacturer recommended feeds, and am only limited by running simultaneously into my machine rigidity, HP and rpm limits, if i get a decent machine with a BigPlus spindle or HSK one day i'll likely be able to push the tools even harder.

 

Also should add that I don't have to worry about paying for tools and my employer is happy for me to push the limits and break a few eggs to make a better omelette 

Message 13 of 13
seth.madore
in reply to: a.laasW8M6T


@a.laasW8M6T wrote:

 

Also should add that I don't have to worry about paying for tools and my employer is happy for me to push the limits and break a few eggs to make a better omelette 


I'm my employer and programmer/machinist all rolled into one 😂


Seth Madore
Customer Advocacy Manager - Manufacturing

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report