Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Custom Tool Lists


Grimes
 Share

Recommended Posts

If anyone knows any old topics post em, couldnt find anything.

 

so in my quest to basically post straight from mastercam into the machine as fast as possible, im now looking at making custom tool lists for different types of materials. i have a very basic one i use but just modified the default one. 

 

trying to keep it simple at first i just want two, one for aluminum and one for like 4140 steel. What i need help with is the speeds and feeds. theses days theres so many different kinds of material and different types of tooling. all the charts and formulas tend to get confusing. looking for a simple(at the start) way to run a tool with speeds and feeds for aluminum and one for steel, so i dont have to modify them after i click the tool.

 

i hope you understand what im getting at..

Link to comment
Share on other sites

This is exactly how I got going creating my custom tool libraries some 20 years ago.

I suggest picking a brand of tools that you like and be consistent. I like widia and helical, so his is always my first choice (add others as needed). When naming tools in library I'm very specific.

 

Example:

.375 DIA EM 4FL W/.875 LOC 1.125 EXT HELICAL HSV-SR-40375 EDP 30322

Keep on adding tools as you go and don't get discouraged! This is a never ending process. Before you know it  you'll have hundreds if not thousands of them in your libraries.

Makes writing toolpaths a snap. It's pretty painful watching some programmers creating or searching for the same tool over and over again.

 

I'd also at the same time add a holder (create an assembly) with the common holders for clearance (1 at a time, as needed). A must when doing multi-axis stuff.

 

You're already ahead of the game by starting this process 👍

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
13 hours ago, Grimes said:

never really messed with the holders, why would it be such an issue other than length of the tool to not crash?

I didn't used to do much with them until I started doing a lot of organic surfacing using a multiaxis.  If you are constantly having to deal with long reach tools and whatnot it's a must to have accurate representation of your holders.  Then once you start doing it here and there it's hard to skip past it, especially if you starting using detailed tool reports.  Going through a report and 5 or 8 holders are defined, the OCD kicks in and you just go ahead and define the rest.  Surprisingly it makes it easier for the operators.  (less decisions)  Another point, if you do your own setups, always, and don't have to have good documentation for other people, then unless there is a reach issue or something where you needed backplot to help determine if it would clear, you probably won't find the value.

Link to comment
Share on other sites

ok this isnt really going where i want it to go, so im gonna just ask what speeds and feeds do you guys run for like a 4 flute 1/2" carbide endmill into 4140 vs. aluminum. and a 1/2" hss drill into 4140 vs. aluminum. i wanna see where im at. our company isnt super high speed machining.

im running around 2000rpm at 15ipm for steel for the endmill, i just basically double them for aluminum. around 500 for the drill at 3ipm, same double them for aluminum.

Link to comment
Share on other sites

Hi Grimes,

If you are looking for advice about what speeds and feed to run, I'd suggest you take a look a the "High Speed Database" that Chris Rizzo started. (Sadly, Chris passed away several years ago, but JP still maintains a copy of the database that is publically accessible.)

Dynamic Database

This spreadsheet contains real world "proven" speeds and feeds that people have successfully run on their machines. The database also gives you info about the setup (sometimes), so you can see what it would take to achieve similar performance.

If you aren't using High Efficiency Machining techniques in your shop, this is a great opportunity to start.

Here are some guidelines if this is new to you:

Steel

  • The Dynamic style paths work best at 2:1 L2D ratio (length to diameter). You can often achieve better performance by switching to a smaller diameter tool, with longer flute.
  • All the following recommendations are for a 2:1 ratio.
  • For Steel start with 15% Radial (Stepover)
  • The Radial Engagement "Range" for Steel is generally: 10-25%
  • As the ratio increases above 2:1, decrease your stepover accordingly. (example: @ 4:1, Stepover should be between 4-8%)
  • At shorter ratios (Ex: 1:1), you can go as high as 30% engagement, but I would consider that the "ceiling" for Steel.
  • For roughing, you should be at 1-2%, "Diameter per tooth", for Feed values.

Example: Cutting 4340 @ 35 RC, on a Matsuura milling machine.

Using a .500 diameter endmill (Titan brand), here are the numbers:

5348 RPM (695 SFM). We engaging the tool radially at 10% engagement (Stepover).

Using 1.25% per tooth (4 flute), we get: 5348 * .0125 = .00625 per tooth. (0.025 per revolution).

0.025 * 5348 = 133.7 Feed Rate

Aluminum

  • Values below assume a 2:1 L2D ratio.
  • Start with 30% radial engagement
  • General range for Aluminum is 15-40% radial engagement
  • Decrease engagement, as length increases. (@4:1, stepover should be between 5-15%)
  • At a 1:1 ratio, you can use up to 45% engagement (although I personally never go above 40% for any tool.)
  • For roughing, you should be at 1.5-2.5%, "Diameter per tooth", for Feed values.

Example: Cutting 6063 Aluminum, on a Mori-Seiki NHX-4000.

Using a .500 diameter endmill (Helical brand) here are the numbers:

12,000 RPM (1560 SFM). We are engaging the tool 30% radially.

Using 1.25% per tooth (3 flute), we get: 12,000 * .0125 = .00625 per tooth. (0.018 per revolution)

0.018 * 12000 = 220 Feed Rate (rounded)  (220 / 12000 = .018333..........3)

  • Haha 1
Link to comment
Share on other sites
1 hour ago, Colin Gilchrist said:

Hi Grimes,

If you are looking for advice about what speeds and feed to run, I'd suggest you take a look a the "High Speed Database" that Chris Rizzo started. (Sadly, Chris passed away several years ago, but JP still maintains a copy of the database that is publically accessible.)

Dynamic Database

This spreadsheet contains real world "proven" speeds and feeds that people have successfully run on their machines. The database also gives you info about the setup (sometimes), so you can see what it would take to achieve similar performance.

If you aren't using High Efficiency Machining techniques in your shop, this is a great opportunity to start.

Here are some guidelines if this is new to you:

Steel

  • The Dynamic style paths work best at 2:1 L2D ratio (length to diameter). You can often achieve better performance by switching to a smaller diameter tool, with longer flute.
  • All the following recommendations are for a 2:1 ratio.
  • For Steel start with 15% Radial (Stepover)
  • The Radial Engagement "Range" for Steel is generally: 10-25%
  • As the ratio increases above 2:1, decrease your stepover accordingly. (example: @ 4:1, Stepover should be between 4-8%)
  • At shorter ratios (Ex: 1:1), you can go as high as 30% engagement, but I would consider that the "ceiling" for Steel.
  • For roughing, you should be at 1-2%, "Diameter per tooth", for Feed values.

Example: Cutting 4340 @ 35 RC, on a Matsuura milling machine.

Using a .500 diameter endmill (Titan brand), here are the numbers:

5348 RPM (695 SFM). We engaging the tool radially at 10% engagement (Stepover).

Using 1.25% per tooth (4 flute), we get: 5348 * .0125 = .00625 per tooth. (0.025 per revolution).

0.025 * 5348 = 133.7 Feed Rate

Aluminum

  • Values below assume a 2:1 L2D ratio.
  • Start with 30% radial engagement
  • General range for Aluminum is 15-40% radial engagement
  • Decrease engagement, as length increases. (@4:1, stepover should be between 5-15%)
  • At a 1:1 ratio, you can use up to 45% engagement (although I personally never go above 40% for any tool.)
  • For roughing, you should be at 1.5-2.5%, "Diameter per tooth", for Feed values.

Example: Cutting 6063 Aluminum, on a Mori-Seiki NHX-4000.

Using a .500 diameter endmill (Helical brand) here are the numbers:

12,000 RPM (1560 SFM). We are engaging the tool 30% radially.

Using 1.25% per tooth (3 flute), we get: 12,000 * .0125 = .00625 per tooth. (0.018 per revolution)

0.018 * 12000 = 220 Feed Rate (rounded)  (220 / 12000 = .018333..........3)

Colin, Would you use these settings using these jaws?

http://www.durusworkholding.com/durus-grip-strip-vise-jaw/

I've attached a file.  If you get a chance, please look at it and give me your suggestions.  This part is 1018, held in those jaws.  Am I, being a CHICKEN with my step over????  I have been looking at the dynamic database, but it doesn't show what the work holding is.

EXAMPLE 1.mcam

Link to comment
Share on other sites

I'll run wildly different feeds and speeds with the same cutter in the same material depending on the specifics of the cut (depth, step, stickout, setup rigidity, etc.).  I use HSMAdvisor and the Helical Milling Advisor to get starting numbers.  As such I never rely on the speed and feed in the tool library, I recalculate for every operation.

  • Like 2
Link to comment
Share on other sites
17 hours ago, Matthew Hajicek™ - Conventus said:

As such I never rely on the speed and feed in the tool library, I recalculate for every operation.

This is me....  I cut wood.  Some would say it's easy.  I'll tell you all otherwise.  It's only easy in that you can rapid a tool through the workpiece and all you will lose is the workpiece.  That's about it.  Feed's can vary based on operation from .002" to .015" per tooth.  Even with the same doc and woc.  It all depends on the setup, and grain direction.  As such I have found that the only useful setting that you usually don't have to play with much is spindle speed.  Some days I wish I could get back to cutting metal, but even in those days, my feeds and speeds were typically set per op, not per tool, too much opportunity for cycle time reduction to leave them alone.  Of course lots of our projects were going run for a few weeks minimum so it was worth the time.  How would you even go about setting up libraries for those cases?

  • Like 1
Link to comment
Share on other sites
On 8/10/2018 at 5:52 AM, Colin Gilchrist said:

Hi Grimes,

If you are looking for advice about what speeds and feed to run, I'd suggest you take a look a the "High Speed Database" that Chris Rizzo started. (Sadly, Chris passed away several years ago, but JP still maintains a copy of the database that is publically accessible.)

Dynamic Database

This spreadsheet contains real world "proven" speeds and feeds that people have successfully run on their machines. The database also gives you info about the setup (sometimes), so you can see what it would take to achieve similar performance.

If you aren't using High Efficiency Machining techniques in your shop, this is a great opportunity to start.

Here are some guidelines if this is new to you:

Steel

  • The Dynamic style paths work best at 2:1 L2D ratio (length to diameter). You can often achieve better performance by switching to a smaller diameter tool, with longer flute.
  • All the following recommendations are for a 2:1 ratio.
  • For Steel start with 15% Radial (Stepover)
  • The Radial Engagement "Range" for Steel is generally: 10-25%
  • As the ratio increases above 2:1, decrease your stepover accordingly. (example: @ 4:1, Stepover should be between 4-8%)
  • At shorter ratios (Ex: 1:1), you can go as high as 30% engagement, but I would consider that the "ceiling" for Steel.
  • For roughing, you should be at 1-2%, "Diameter per tooth", for Feed values.

Example: Cutting 4340 @ 35 RC, on a Matsuura milling machine.

Using a .500 diameter endmill (Titan brand), here are the numbers:

5348 RPM (695 SFM). We engaging the tool radially at 10% engagement (Stepover).

Using 1.25% per tooth (4 flute), we get: 5348 * .0125 = .00625 per tooth. (0.025 per revolution).

0.025 * 5348 = 133.7 Feed Rate

Aluminum

  • Values below assume a 2:1 L2D ratio.
  • Start with 30% radial engagement
  • General range for Aluminum is 15-40% radial engagement
  • Decrease engagement, as length increases. (@4:1, stepover should be between 5-15%)
  • At a 1:1 ratio, you can use up to 45% engagement (although I personally never go above 40% for any tool.)
  • For roughing, you should be at 1.5-2.5%, "Diameter per tooth", for Feed values.

Example: Cutting 6063 Aluminum, on a Mori-Seiki NHX-4000.

Using a .500 diameter endmill (Helical brand) here are the numbers:

12,000 RPM (1560 SFM). We are engaging the tool 30% radially.

Using 1.25% per tooth (3 flute), we get: 12,000 * .0125 = .00625 per tooth. (0.018 per revolution)

0.018 * 12000 = 220 Feed Rate (rounded)  (220 / 12000 = .018333..........3)

I saw the DYNAMIC DATABASE through GOOGLE SHEET.  I saw some funny comment as "

 

"I F***** UP" and... "TMAO" hahaha....., who created those?

Link to comment
Share on other sites
On 8/10/2018 at 8:52 AM, Colin Gilchrist said:

but JP still maintains a copy of the database that is publically accessible.)

Just to clarify, I do not....what's available is Chris's, what he created and shared...

Link to comment
Share on other sites

finally im back reading through all the replys, thanks everyone. jp that was what im looking for to start(18000 wow my new machine goes to 10000, old one i dont run above 6000), and colin for what i want to advance to. Our shop is basically still running in caveman times. im trying to learn all these new toolpaths mastercam has(im still taking .05" depth of cuts), and surprisingly i know mastercam better than everyone in our company and i know nothing compared to people on this forum. matthew i downloaded HSMAdvisor thanks, have to figure it out at work.

 

again, thanks everyone!

  • Like 2
Link to comment
Share on other sites
On ‎8‎/‎10‎/‎2018 at 10:16 AM, Roger said:

Colin, Would you use these settings using these jaws?

http://www.durusworkholding.com/durus-grip-strip-vise-jaw/

I've attached a file.  If you get a chance, please look at it and give me your suggestions.  This part is 1018, held in those jaws.  Am I, being a CHICKEN with my step over????  I have been looking at the dynamic database, but it doesn't show what the work holding is.

EXAMPLE 1.mcam

Hi Roger,

Sorry I missed this when you originally posted it. I'll see if I can find some time tonight or this weekend to throw down some sample paths.

The quick answer to your question is this: you need to keep the stepover small! It is the feedrate that you need to kick up!

Those samples in the HSM database could really benefit from some "setup" info, but your dovetail jaws should be plenty strong for holding purposes. I would just recommend that you leave enough of a "floor" to make sure the setup stays rigid as you remove material.

What do I mean by "floor"?

As you machine the part out, there will be material that is left underneath the part, that is still being gripped by the jaws, and is still supporting the part.

My general rule is a 10:1 ratio between "floor thickness" and "span" between the jaws. So, for every "1 inch of span" across the jaws, leave yourself ".100 of floor" below the part.

Now, I've violated this guideline plenty of times, as the situation dictated, but I typically paid the price in the form of chatter. This then necessitates slowing down the paths, and the price you pay is lower productivity. For prototype or small lot sizes, the time is negligible. For larger runs, I will typically leave that "10:1" floor, and do all my heavy roughing, and semi-finishing. Then I'll relax the part, re-clamp, and add some additional "roughing" paths to reduce the floor thickness. Typically I'll use a High-Feed style cutter for this, because it directs the cutting forces up into the spindle, and (relatively speaking) has a lower cutting pressure on the part itself.

For 1018 Steel, I'd recommend a 12% Radial Stepover value. There is no need to "maximize" the radial stepover value. I prefer to keep my stepover values conservative, and simply increase the Feed when I feel like there is more performance to be had.

When we create a HEM path, Mastercam still has to vary the cutting width just a little bit. (Their algorithm is good, not perfect!) So, as the cutter is engaged, going around the contour being created during roughing, the tool is not only entering/exiting the material, but you'll notice that the tool will engage "more material radially", as it goes around external corners in the path. For this reason, I tend to stick with conservative radial values, to ensure that I don't overload the cutter and get catastrophic tool failure.

For your particular setup, I'd start with the following:

1018 Steel = 600 SFM

Tool = .500-DIA, 1.625-LOC, 4.0-OAL, 4-FLT (Helical HSV-M-40500, EDP: 30542) Note: there is a 2nd EDP #, which includes a Weldon Shank Notch: 30542-W

With that tool, it makes a difference how deep you are cutting as well. Our max depth is 300% of the diameter. (1.500 DOC)

All numbers use 4576 RPM (597.6 SFM)

With 0.750 DOC                               With 1.000 DOC                                With 1.500 DOC

Fz=.0045 (81.83 ipm)                      Fz=.0034 (61.37 ipm)                        Fz=.0022 (40.92 ipm)

  • Like 1
Link to comment
Share on other sites
  • 1 year later...
8 hours ago, M4573RMZD said:

I came across this thread but I cannot get the "Dynamic Database" The link is gone.

It's in the pinned important topics thread.  But appears to be broken.  I guess we will need to see if JParis can resurrect.  This came up the other day and I regret I don't recall if a new link was made.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...