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:

Tool Ø recommendation to cut a slot using dynamic roughing...


Watcher
 Share

Recommended Posts

Hi folks,

 

Wel, as you know I´m not a Mastercam user any longer so Dynamic Milling is not something I have at my disposal...

 

However, we´re rehearsing to play with Volumill to cut some slots in Inconel 625... the idea is to perform cuts at full depth (1") with an endmill...

 

The slot width is 1", and I´m all ears for suggestions about the Ø of the tool to cut this using a dynamic toolpath like Volumill (Dynamic Milling in MC)... I´m thinking about suggesting our programmers to start with 20mm endmill (0,787"), 6 flutes. I have read the "Inconel" posts and I´m considering high-end tool holders (Corogrip 930 / Shrink-Fit) and also high-end endmills like Hanita Varimill, Iscar Chatter-Free, Jabro Tools...

 

So the point is really about how wide (Ø) the tool should be in order to allow the algorithm to generate the required moves so that we have proper chip evacuation while we have the biggest possible Ø (And thus stiffness) in the tool?

 

Scenario:

  • Slot is like an obround, but one end is open (The side we will approach the material)
  • The width of the slot is 1" and the length is 5"
  • Inconel 625
  • 28 slots per part
  • Full depth of cut is the dream (1" DOC)

 

I´m all ears for suggestions and approaches...

 

Tks in advance,

 

Daniel

  • Like 1
Link to comment
Share on other sites

Got the RPM for ceramics?

that's your best bet, otherwise buy a big container for scrap carbide.

If not, I have had very good results with Seco jabra highfeed endmills. I only take about .02 depth of cut but I am able to run at 20 to 25 IPM at 125 SFM

  • Like 1
Link to comment
Share on other sites

I would look at using a 5/8" (or 16mm) tool for that.

The problem with a 20mm tool would be that it is too close to the slot width so to keep the engagement angle down (and heat) you would have to reduce your step over.

But too small a step over and then the heat becomes an issue because on hi-temp alloys it's best to keep a good chip thickness (which I'm sure you know already).

 

Also I've found that it is best to keep this type of toolpath to a maximum depth of 1.5 x tool diameter so 16mm just fits with that (little bit over I know).

5%-10% stepover, I'd start at 5% and see what the cycle time vs. tool life analysis comes out at.

 

Mitsubishi, Jabro or Hanita (in that order) are the tools for this in my opinion.

 

And as high pressure a coolant flow as you can get on it, seriously the higher the better.

Link to comment
Share on other sites

my first choice would also be Ø1/2" as a sweet spot in price and performance. 20mm would be way too close to slot width where you would end up with large angles of engagement thus bigger forces.

using a ceramic insert cutter at crazy high RPM's seems like they work on YouTube and have heard confirmation with colleagues as to the veracity of this shallow axial technique. this would allow you to use old sckool gouge it out toolpaths that you already have access to and might just be faster.

Link to comment
Share on other sites

Daniel,

 

14mm Is probalby going to be your best choice the percentage of step over is going to be key here as already suggested. I suggest taking the 25mm depth and make it as 12.5 mm depths of cut and stay in the SFM recommended for the cutter. Be instresting to see how what Mastercam has would do in this application.

 

Keep us posted on what you come up with.

Link to comment
Share on other sites

Hi folks,

 

Thank you very much for all responses so far. Fortunately/unfortunately I´m no longer a NC-Programmer in my day-to-day work, but I do support them technically and you guys know I have coolant running on my veins too, even working more on the IT/Technology side of the thing now...

 

I´m trying to take my aerospace background to the Oil&Gas segment, as we are a very conservative niche of the industry in regards new methods. I´m coaching a couple of old school programmers to take the best of our WFL Millturns...

 

The test is planned for somewhen around June... so now I´m kind of researching and helping them to procure tooling so that we have the best resources at our disposal when we push the green button.

 

I´m really trying to stay away from ceramics as I want to prove my point that carbide and the right algorithm can make miracles when properly applied... I´m more interested in the HPM side rather than HSM. They don´t believe when I say we can cut Inconel with a 1" depth using a 16mm endmill... I want to show them the beauty of the science... I´m kind of tired of the "Guy that used to cut aluminum" jokes... :D

 

Thank you everybody, I´ll keep ya posted!

 

Ron, I did not forget you my friend.. just going through a busy period - (Got back to the college... IT this time :D)

 

Daniel

Link to comment
Share on other sites

Daniel, I figured as much and a 16mm should probably do it, but go with a 5 flute for core strength. I have used 8 and 10 flute endmills on high RC materials for finishing with great success but here think it will do more harm than good. You need all the chip clearance you can get and core diameter on the endmill. Thing people forget about with the more flutes is the core diameter of the endmill get much smaller. Without the core you do not have the strength needed to even try something like this on such a hard material. It is nice sometimes to show people yes I can walk the walk and not just talk the talk.

 

Catch up with me when you can. :geek:

Link to comment
Share on other sites

I believer the default rounding radius in Volumill is 45%. Although very smooth it's not suited to all conditions as this forces a cutter diameter selection small enough to fit those parameters, may lead to a diameter to length ratio that is less than optimum, and may require multiple axial passes as well as more rest milling. It can be over ridden to suit the tooling on hand. Volumills allegiance with Helical Solutions has produced a speeds and feeds app that boast some pretty impressive data. IMO, it's worth a look. http://www.millingadvisor.com/

 

Although I don't machine the high temp alloys, Chris Rizzo recommended a 30% rounding radius as a rule of thumb with this style of machining and it has worked very well in both MC and Cimco/HSMWorks products for me.

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...