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:

High Feed Machining

Longbow

By Longbow,
in Industrial Forum

 Share

Recommended Posts

Longbow Newbie

Longbow

Posted
Posted

I know this topic comes up often. Ive looked thru the history and havent found much on it that will help so Im going to bring it up again. I have two Fadal machining centers and I have my high feed option set but its not what it should be. Is there anyone out there with settings for Fadal or someone that can tell me how to optimise it? I would like to use it on roughing also for slowing down when feeding in a "-" motion and speed up when in a "+" direction.

Link to comment
Share on other sites
Mike Whitten CAD/CAM Contractors Newbie

Mike Whitten CAD/CAM Contractors

Posted
Posted

Longbow,

 

Do this: read all of the help on it and try some examples. It takes some playing with but you will get it.

What do you mean by this:

quote:
also for slowing down when feeding in a "-" motion and speed up when in a "+" direction.

I can post up some example files later if you want and also help more but I am on a hot job right now. Let me know.

 

Mike

Link to comment
Share on other sites
Longbow Newbie

Longbow

Posted
  • Author
Posted

What do you mean by this:

 

quote:

--------------------------------------------------------------------------------

also for slowing down when feeding in a "-" motion and speed up when in a "+" direction.

--------------------------------------------------------------------------------

slowing down when it plunges in a z negitive and speeding up wing cutting in a z positive motion.

 

 

Yes if you have an example or two to share it would be great.... its getting better but not there yet.

Link to comment
Share on other sites
Mike Whitten CAD/CAM Contractors Newbie

Mike Whitten CAD/CAM Contractors

Posted
Posted

Longbow, it will work good for that. You just have to spend some time on it. There was a good thread on Highfeed about a month ago. Try to search for it.

 

I put a roughing example in the MC9 files directory for you.

 

"Highfeed example from Mike Whitten.MC9"

 

What is so good about Highfeed is that it is very flexible and can be manipulated to get what you want.

 

Thanks,

Mike

Link to comment
Share on other sites
wildcat99 Newbie

wildcat99

Posted
Posted

Search for thread topic "highfeed help". You will find some very good information here. I cut my first highfeed part a few weeks ago, with help from this forum, and it worked great. Aluminum chips were flying everywhere, and I didn't have to touch the feed override knob because it slowed feed where it needed to.

 

There are a lot of variables that affect how fast you can cut a part, but like Mike said you can make adjustments in highfeed to get what you want.

quote:
slowing down when it plunges in a z negitive and speeding up wing cutting in a z positive motion

On the Material Removal Rate page in highfeed, at the bottom there is an "up feedrate scale factor" and a "down feedrate scale factor" that will do exactly this.

 

I still have some tweaking to do with highfeed and will have a chance to experiment on 2 more aluminum parts when I get machine time. Two things that I keep in mind when using highfeed are:

 

1. Highfeed will cut as fast as possible when it can, but slow down when it has to.

 

2. The worst that can happen is I will have to turn the feed override knob down. cheers.gif

HTH

Link to comment
Share on other sites
Longbow Newbie

Longbow

Posted
  • Author
Posted

Thanks Wildcat that is exactly what I was looking for. Im running all A2 and other tool steels and the plunge was wearing my hand out on the feedrate knob. I'v got the part on the finishing working great. I cant wait to try the roughing part now. If anyone needs the settings on the high feed for finishing on a fadal Ive got some numbers that work really well... running 200 inches a minute right now and as smoothe as silk, cut my machining time in half on this job.

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
Posted

quote:
If anyone needs the settings on the high feed for finishing on a fadal Ive got some numbers that work really well... running 200 inches a minute right now and as smoothe as silk

I'd be interested in those settings also! High feed is another thing on my "things to learn about" list. We cut mostly A2, D2, etc tool steels also. We cut some at 130 IPM, but 200 IPM would be even better!

 

Thad

Link to comment
Share on other sites
Longbow Newbie

Longbow

Posted
  • Author
Posted

This is working for me now... still tweeking on it but have had great luck with it. Finishing only ... I will be playing with the roughing today.

 

Recombine segments when feed rate changes less than (%) = 10.0

 

Look ahead(as a % of tool diameter)= 100.0

 

Maximum feed rate change per block= 30.0 (still playing with this one alittle to try to speed it up more.

 

CHECK Accelerate to smooth feed rates

 

Segment length (%of tool diameter) = 15.0

 

Slow down to mimimum cornering feed rate when direction changes (degrees) = 45.0

 

Mimnimum cornering feed rate = 20.0

 

Cornering acceleration in Gs = 0.01

 

You Fadal guys try these out and let me know what you think.. if you find something that works better let me know and Ill do the same.

Link to comment
Share on other sites
Longbow Newbie

Longbow

Posted
  • Author
Posted

I just ran it on a roughing operation. It cut the machining time from 43 min. to 22 min. The stock set up part is great. I saved an STL file and used it for Stock Setup and it knew when it was cutting air and rapided thru that part and full cut was my programmed feed rate and would speed up and slow down depending on the engagement of the tool. It was awesome.

 

As far as the dongle no I cant take it home. We have only one 3-D one and its used alot by others desinging and such. I dont think he would let me take it home anyway. I have considered buying it myself for some design work I do at home on my recurve bows but hard to justify the cost for a hobby.

Link to comment
Share on other sites
Longbow Newbie

Longbow

Posted
  • Author
Posted

In the help section it says that the cutter comp will not work with the highfeed machingin...

From Mastercam Help FIle:

 

Intended use

 

¨ Works with 2.5-axis and 3-axis toolpaths.

 

¨ Applies only to machine moves specified by G0 – G3 codes

 

¨ Works with flat, bull, and ball cutters.

 

¨ All selected operations must use the same tool plane.

 

¨ Does not work with 5-axis toolpaths.

 

¨ Does not modify feed rates when cutter compensation in control is used.

 

¨ Does not handle position codes.

Link to comment
Share on other sites
gcode Experienced

gcode

Posted
Posted

quote:
Does not modify feed rates when cutter compensation in control is used

I was using "wear" comp, which is the same as

"computer" with G40's and G41's added at the

right spots. It my case the G41's are being added

to G03 moves.

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...