A little OT....cool video

[Roger Peterson]

It appears the HFF has a couple of issues in X4 as it's not recognizing the material removal rate and it uses the air cutting rate for in material cuts. But it works well just using in "finishing only" mode as it will slow it down whenever there is direction change. This does require "tweaking" the machine dynamics away from what the machine is capable of and set them to what works for that particular operation.

 

 

The end result is that you have a dynamic mill toolpath that slows down on a direction change so the tool load is much more stable on those first few passes on the outside corners.

 

 

Regards,

[MIL-TFP-41]

The dynamic mill sample file also does the exact same thing that Neurosis is talking about. On the first pass...on the first corner the tool is engaged by almost .420 (84% engagement!!)....way more than the .25 (50%)specified in the cut parameters

 

[David Conigliaro CNC Software Inc.]

OK guys, I haven't cut titanium with Dynamic Mill yet. But, this condition you highlight has not broke a tool in 35Hrc P20 on me yet for example. I've been cutting with, say a 1/2 endmill, 1 inch deep no stepdowns. But I use a very small stepover never more than 10%DIA and very high feedrates and spindle speeds 300-700IPM 5000-12000RPM. And yes my MRR's are higher than they would be if I was programming at traditional stepovers and traditional feeds. Better tool life as well.

 

Will this condition be more evident in the titanium world, if so, any other materials?

 

Give me some cut conditions and speeds you succesfully use for titanium.

[neurosis]

Here in the next week we will be starting this titanium job. I will be running the feed rates at up around 110 ipm @ 1" D.O.C. I will be using Volumills path to run the part as I am confident in the results we have had with it so far. I can enter the same parameters in to the Dynamic Milling and try to run a part if you are confident that it will not break the tool. So far we have only tried this in the stainless and have been apprehensive about trying it in titanium. We were cutting 1.25 deep with a .05 radial in the stainless at 133 ipm.

 

The path shown in my picture above is set for a .035 step and in the corners it raises up to .110. This is using a 1/2" endmill as well.

[Roger Peterson]

When your roughing tool are roughing with tools 1mm or .5mm and finishing with as small as .1mm the little "tink" sound is easy to come by...

 

50-52rc 420 stainless is pretty common.

 

If you haven't done much testing using "small" tools, that would be a good place to start.

 

anything medical requires small tools, stints, pacemakers, defibs, hearing aids, bone screws, etc...

regards,

[Glenn Coleman]

Neurosis,

 

There are a couple of settings you should know about when machining titanium (or other hard materials) with VoluMill. Be sure to check the “Side-mill only” checkbox at the lower-right of the “VoluMill parameters” dialog. This will ensure that no slot milling takes place anywhere in your toolpath. Then, as an option, you may want to check the “Side-mill stepover” box in the “Slot-mill/side-mill overrides” frame. This will allow you to enter a smaller stepover value to be used in the tighter areas of your part, such as when working into corners, necks, and other narrow areas.

 

 

 

I used .025 in this example, based on the.035 stepover you mentioned in your post. This is an example only. Using this option will lessen the load that would otherwise be in play in the tighter areas of your part. We have found that values in the neighborhood of 1/2 to 2/3 of your main stepover to work well in materials such as 17-4, 15-5, and 304 stainless. For softer materials such as aluminum, it is usually not necessary to override your main stepover.

[neurosis]

Glenn,

 

Absolutely! I used the same settings for the stainless as well. I was running so fast that I couldnt afford to have it channel anywhere. I'll give it a shot with the adjusted side-mill stepover. When I ran the stainless I never adjusted that value and it worked beautifully. I did have to play with the smoothing radius to get it to clear out some of the tighter corners.

 

I am looking forward to trying this out in the TI. If I can get a vote of confidence from Dave on the Dynamic Milling, I wouldnt mind running a head to head on the two paths and compare some tool life results between the two.

[David Conigliaro CNC Software Inc.]

Neurosis:

quote:

---

I was never able to get the Dynamic Milling to control the tool engagement when entering the stock which would break the tool in the first cut. Once the Dynamic Milling was able to remove enough material to create its race track it looked good but I was never able to get that far in to the part using it.

---

First was the shape your cutting a core entering from outside or a cavity ramping in? If it was acavity ramping in did you use the entry settings? You have control over your ramp angle or pitch, RPM, IPM, even a dwell to allow the spindle to transition from your entry speed to your cutting speed if needed.

 

[MIL-TFP-41]

David,

 

You should write a short tutorial on using all of these settings.....This thread has got a lot of useful information on the Dynamic mill toolpath....and I am sure most could benefit from a short .pdf or powerpoint on using all of these settings.

[neurosis]

Dave,

 

It was exactly as the example shown in the picture that I posted. It was a core style roughing of a profile. No ramping involved. I mis-spoke when I explained the problem. The path didnt have an issue until it hit the corner and over-engaged the material.

 

[ 07-07-2009, 11:09 AM: Message edited by: Neurosis ]

[David Conigliaro CNC Software Inc.]

Thanks Neurosis

[mig]

so it going to be change on next MU?

[neurosis]

I set up two paths on the same profile today. One using Cimco's Adaptive Clearing, and the other with Dynamic milling. The two paths look almost identical except that the Adaptive clearing path ran the endmill further along the edges prior to rounding at the corners. Cimco's path did not over engage the tool in the corners as the Dynamic Milling does. It looks like there may be a little room for improvement where the corners are concerned?

[Roger Peterson]

a max stepover value would be effective

 

 

How about dynamic restmill???...

[Pat Martucci CNC Software]

[ 07-09-2009, 09:39 AM: Message edited by: Pat Martucci, CNC Software ]

[neurosis]

I wanted to bring this back up because the question of the tool being over engaged in corners being changed in future releases was never answered. Is this something that will be looked in to?

 

Will there eventually be a 3d dynamic milling?

[David Conigliaro CNC Software Inc.]

Neurosis - We are currently looking into the corner overload condition. Alot of things are kicked around for the future,a public forum is no place to communicate what we are working on....competitors watch this forum

[Guest CNC Apps Guy 1]

quote:

---

...competitors watch this forum...

---

Like hawks. How do you think their demo jocks know EXACTLY what to show t ohighlight their strengths against Mastercam? It certainly isn't because they are better. They merely do their homework, in here.

[neurosis]

quote:

---

Neurosis - We are currently looking into the corner overload condition.

---

That was all that I really wanted to know. After talking to you and playing with this path a little I can see where it will come in useful. I like the amount of control that it gives you.

 

Thanks.

[thanhsonnguyen]

guru i'm love that too

[Glenn Coleman]

I am happy to report that the lawsuit between Celeritive and Surfware has been dismissed. For the formal statement, please visit our website at http://www.celeritive.com/company-news.htm. Also note on our News and Events page that we have released VoluMill 3.0, which includes VoluMill for 3-axis roughing, and several enhancements to our 2-axis product.

 

Thanks,

[Colin Gilchrist]

Cool, good news Glenn.

 

FYI, the link you posted has a period at the end, which gives a "Not Found" error. You might want to go back and edit the link.

 

fixed link

[Rob @ Target Machine]

Thanks Colin.

[Glenn Coleman]

Sorry, the link should have been:

 

http://www.celeritive.com/company-news.htm

 

Thanks,

[Joe788]

quote:

---

Also note on our News and Events page that we have released VoluMill 3.0, which includes VoluMill for 3-axis roughing, and several enhancements to our 2-axis product.

---

Damnit! I had a big chunk of change all set aside to buy the fancy In-House Variaxis post in a few months, and now you throw this at me. The 3 axis roughing product looks outstanding.