HSM on a Fadal.

Atomkinder · Oct 19, 2014

At work we've got two machines currently: A Haas VF-6SS and a Fadal VMC2216. Now the Haas will keep speed quite well, but I'm attempting to increase things such as tool life while either retaining or shortening cycle times. We make a lot of different parts, all for in-house products, so most runs are under ten parts, but we have a couple that I think would benefit greatly from some HSM paths, and the previous programmer did a garbage job of utilizing flute length, so we see a ton of end mills wear out the first 1/8" while the remainder sees almost no use.

The question here is: will the Fadal be able to handle some moderate HSM paths in mostly mild steel parts? Talking 60ipm with G8 turned on and leaving .02-.05" for finishing stock. I've been fairly impressed with it for a Fadal so far, and the G8 feature, so I'm hoping to get some return out of this investigation. I will be trying a path on some excess material tomorrow with an air blast on an AlTiN 4-flute, hot rolled steel, nothing special, but we rarely deal with special anyway.

Anyone tried this? Or do this regularly?

scadvice · Oct 19, 2014

U tube.

HSM on a Fadal - YouTube

dstryr · Oct 19, 2014

The fadal isn't that bad where you need to leave .020 stock at only 60 ipm.
I rough parts on my Fadal in g8 at 150-200 ipm. I leave about .010 stock and have never had issues with overcutting.

Atomkinder · Oct 19, 2014

dstryr said:
The fadal isn't that bad where you need to leave .020 stock at only 60 ipm.
I rough parts on my Fadal in g8 at 150-200 ipm. I leave about .010 stock and have never had issues with overcutting.

This is what I wanted to hear

Dave K · Oct 19, 2014

Wow, a thread about Fadal with no one trashing the machine. About time.

dstryr · Oct 19, 2014

Dave K said:
Wow, a thread about Fadal with no one trashing the machine. About time.

My 2216 ate a belt on Saturday....bastard POS machine

Northwestfab · Oct 20, 2014

We can leave .005-.01 for a finish pass using HSM and/or high feedrates (not in a straight line) and the part will clean up. That said, the heavy tables and not so elegantly tuned servo parameters can hammer the shit out of the thrust bearings. Our lighter EMC seems to do better in this regard, possibly due to the lighter weight and linear guides, the 4020 slams itself around a fair bit.

We need to try some of the volumill paths that leave the machine in G1, switching from G1 to G0 adds an extra hesitation when it isn't necessary.

Atomkinder · Oct 21, 2014

Ran the path today. Unfortunately the code is a crapload of short line moves so it still stuttered on occasion, but G8 kept it mostly moving quickly. Tool looked great (which was the point: extending tool life and finish quality over a run of parts).

On another note when I was checking the code I found something else super fun about the Fadal control: Isometric program backplot! With zoom even! Every time I look around a bit more in that control I find something else new and awesome from 1997 that I don't even see on the machine made in 2012.

Dave K · Oct 21, 2014

Every time I look around a bit more in that control I find something else new and awesome from 1997 that I don't even see on the machine made in 2012.

That control is awesome to me. I know it's old school, but it's old school with just about every option that could have ever been available on a control like that. And the best part is, it all came standard with that control. I love all the ways to edit stuff. Multi edit, starting the control at any given point, mass delete, copy and paste, etc. And the little macros that are there for picking up edges, and measuring tool lengths makes it all quick and easy.

Bobw · Oct 22, 2014

dstryr said:
My 2216 ate a belt on Saturday....bastard POS machine

Mine ate one a few weeks ago.... Here is the 2 belts after removal, one of them went into the "good enough in an emergency" pile, the other in the trash.

realsquash · Oct 23, 2014

I do it all the time on a 2216. I even DNC it at 19.2kbps because the control has so little memory. After using HSM paths there is no way I would ever go back. Even a 3hp knee mill makes good time with HSM paths when you don't have to baby it in corners and the like.

Silent_Man · Oct 23, 2014

Atomkinder said:
Ran the path today. Unfortunately the code is a crapload of short line moves so it still stuttered on occasion, but G8 kept it mostly moving quickly. Tool looked great (which was the point: extending tool life and finish quality over a run of parts).

On another note when I was checking the code I found something else super fun about the Fadal control: Isometric program backplot! With zoom even! Every time I look around a bit more in that control I find something else new and awesome from 1997 that I don't even see on the machine made in 2012.

You need to do set an arc filter to get rid if the short line segments. I presume you are DNCing the program, in which case there are a couple excellent MMS articles online to read up on.

Silent_Man · Oct 23, 2014

Found them. I copied and pasted from this thread:
http://www.practicalmachinist.com/vb/showthread.php?t=287223

Silent_Man said:
Remove block numbers and spaces. This will reduce the data to transmit by a significant amount. 
 
MMS has a really good article on this as well: 
http://www.mmsonline.com/articles/dnc-faster-and-better----part-one 
 
http://www.mmsonline.com/articles/dnc-faster-and-better----part-two

Atomkinder · Oct 23, 2014

Silent_Man said:
Found them. I copied and pasted from this thread:
Dealing With Drip Feed Data Starvation

No DNC, but I will certainly read up on it.

Atomkinder · Jan 21, 2015

Bringing this one back. Today I reprogrammed a part that previously used a 1-1/2" 3-flute insert mill for a roughing operation followed by a 1/2" end mill to clean up and finish. Now it uses one 1/2" end mill for the entire profile. Set the RPM at 6000, .05" rDOC, .75" aDOC, .0048/flute and fed at a nominal rate of 115.2 IPM with Volumill, with a backfeed of 200 IPM. Wish I could take a video, but almost all the parts made in house are intellectual property and hence, no photos or video. The machine handled it quite well, very little stutter, nice blue to gold chips. Material was hot rolled mild steel, probably 1018/1020 or the like.

Coworker said he had never seen the Fadal run that fast. I told him it likely never has!

Edit: left .01" for a finish, and it all cleaned up.

adama · Jan 21, 2015

I do a job on my cnced bridgeport, (vari speed 2hp head) 45HRC steel wear plate, carbide 6mm 3 flute end mill cutting 6mm deep 0.6mm step over, hsm speeds but at bridgeport levels! its not fast but i get a lot of bits and a lot of metal removed from the end mill. Whats more all 6mm of the 8mm flute length is stuffed by the time its had enough. I also use a lot of HSM type paths as std now. I can reliably go 1" deep in a single pass with a Hss coated 1/2" milling cutter and only get 1 thou of taper in mild steel. Whats more with no step wear the cutters make a nice finish and keep a nice finish for ages and ages. HSM - full flute length cutting has to be the best tip i ever read on this forum. Its saved me a ton in cutters over the last couple of years + made better parts.

aarongough · Feb 5, 2015

Atomkinder said:
Bringing this one back. Today I reprogrammed a part that previously used a 1-1/2" 3-flute insert mill for a roughing operation followed by a 1/2" end mill to clean up and finish. Now it uses one 1/2" end mill for the entire profile. Set the RPM at 6000, .05" rDOC, .75" aDOC, .0048/flute and fed at a nominal rate of 115.2 IPM with Volumill, with a backfeed of 200 IPM. Wish I could take a video, but almost all the parts made in house are intellectual property and hence, no photos or video. The machine handled it quite well, very little stutter, nice blue to gold chips. Material was hot rolled mild steel, probably 1018/1020 or the like.

Coworker said he had never seen the Fadal run that fast. I told him it likely never has!

Edit: left .01" for a finish, and it all cleaned up.

Very glad I found this thread! My new VMC10 will hopefully be getting run pretty much exclusively with HSM toolpaths as I'll be doing low volume production.

How are you getting the toolpaths onto your machine currently? You said you're not running DNC so that piqued my curiosity...

Atomkinder · Feb 5, 2015

aarongough said:
Very glad I found this thread! My new VMC10 will hopefully be getting run pretty much exclusively with HSM toolpaths as I'll be doing low volume production.

How are you getting the toolpaths onto your machine currently? You said you're not running DNC so that piqued my curiosity...

Standard RS-232 cable transferring the file as a whole. We don't keep any programs in the machine so all 472k is free. We run a lot of simple parts and program files are typically under 50k. What was being referenced was a drip feed though, in which the control runs from the program directly over the RS-232 without storing it. Works well if the program is too big for control, but I've never actually had to do it.

What will you be using for CAM?

aarongough · Feb 5, 2015

Atomkinder said:
Standard RS-232 cable transferring the file as a whole. We don't keep any programs in the machine so all 472k is free. We run a lot of simple parts and program files are typically under 50k. What was being referenced was a drip feed though, in which the control runs from the program directly over the RS-232 without storing it. Works well if the program is too big for control, but I've never actually had to do it.

What will you be using for CAM?

Ok cool, that sounds very reasonable. I hadn't really considered that I might be able to *not* drip feed the machine but I guess I have no idea yet how large my programs will be!

I'm planning to use HSMExpress for most of my CAM. I have a couple of programs I can use though: Vectric Vcarve Pro (intended for CNC routing but works fine for a lot of milling too), HSMExpress and another one called MeshCAM that does 3D 3&4 axis toolpaths. Will likely stick with HSMExpress for the most part as I design my parts in SolidWorks, when I have to do a 3D toolpath I'll likely have to use MeshCAM for the moment as I can't afford HSMWorks.

Atomkinder · Feb 5, 2015

We use CamWorks with VoluMill at work, but I did get the IT guy to install HSMXpress on 'my' computer and I do like its versatility much more (plus I use Fusion 360 at home, same paths). It does a lot of point-to-point code though, so you'll have to play with the smoothing and tolerance settings to get it to play the nicest. I'd avoid the Vertical Lead-ins, too, unless truly necessary for floor quality.

HSM on a Fadal.

Titanium

Titanium

Diamond

Titanium

Diamond

Diamond

Aluminum

Titanium

Diamond

Diamond

Aluminum

Aluminum

Aluminum

Titanium

Titanium

Diamond

Stainless

Titanium

Stainless

Titanium

Similar threads