A little OT....cool video

[Guest CNC Apps Guy 1]

Better ©opyright it so you can cash in !

[Rob @ Target Machine]

I'm working on that right now, but it's got so many bugs. I guess I'll fix them in the Mu1. LOL

 

 

[Roger Peterson]

If you check the box for open pocket machining you can "core rough" using the dynamic mill function where it starts from the outside and works its way in.

[David Conigliaro CNC Software Inc.]

I'm the product manager responsible for Dynamic Mill at CNC Software. I have been cutting with Dynamic Mill for well over a year. I'm aware of Volumill and Surfcam's technology's as well. I'm willing to look at any file or part any of you are having trouble with or questioning the motion of using Dynamic Mill. Sometimes it could be a lack of understanding of the chaining techniqes, when to use the "Open machining method", bad settings, or the toolpath needs improvement somewhere. Regardless, all the above discussion is good, however, I need you to help me, I need part files, examples, wishes, communication other than "it failed" or the other guys were better. I'm willing to take all your feedback and information and make Dynamic Mill better.

 

Are any or your shops in Michigan?

[Leigh @ Kodiak]

David, any tips on how to get a bull end tool to clean up properly where two regions meet?

[David Conigliaro CNC Software Inc.]

Send me an example, we have discussed bull nosed tools.

[Rob @ Target Machine]

I wasn't aware that Dynamic Mill was capable of open pocketing. Sounds good.

 

Is there a way to control radial engagement, not just stepover?

 

I'll be buying X4 Mu1 for myself in the fall.

My boss won't buy again because X1 was so buggy. I guess he feels burned.

 

I look forward to sending some feedback.

[David Conigliaro CNC Software Inc.]

You cannot control the engagement via an engagement angle setting. But, the motion generated will be safe to run similar to how Volumill doesn't program with an engagement angle. Just have a look at the backplots, you'll see safe, consistent motion. I've cleared P20 pockets with isalnds and such cutting 1 inch deep with a 1/2 inch cutter at over 700 IPM safely on Makino's and Okuma's.

[Rob @ Target Machine]

Thanks Dave - Maybe I'll look into breaking a CD early to get my own seat a little sooner.

 

I'm all done waiting for the company to buy X4.

[cobra95kev]

I think if they use engagement angle that would trigger an immediate lawsuit from Surfcam. It will be interesting to see how that lawsuit linked to above plays out. It is too bad Surfcam has such a tight lock on that because it is awesome in hard metals.

[neurosis]

quote:

---

I'm the product manager responsible for Dynamic Mill at CNC Software.

---

Is the dynamic milling supposed to be capable of a core style roughing at this time? I was able to get it to core rough exactly how Roger stated above. I wasnt sure if it was meant for that, but if it is, I can show you some pictures of the issues that I had with it. IF not then... Will there be a core style roughing using dynamic milling in the future?

 

And mastercam guru, can you shrink that picture a little... its tooooo big.

[David Conigliaro CNC Software Inc.]

Neurosis - Yes it is capable of core style machining. Only from the standpoint of machining the identical part you would use core mill for. It will not take a bunch of open cuts, it uses a more efficient approach. Any part you have used core mill on can be switched to a Dynamic mill on the tooltype page, you just have to check the 'open machining method' check box on the cut parameters page to put dynamic mill inito a core mill train of thouhgt. We are considering breaking Dynamic Mill into two toolpaths for X5 "Dynamic Core Mill' and Dynamic Area Mill'. You have those two toolpaths today via the 'open machining method' check box.

[Rob @ Target Machine]

How about chord length?

 

That's a function of, but not, per se, the engagement angle.

 

I don't see how basic machining principles can be copyrighted.

 

The intellectual rights of a programmer/developer don't need to include machining methods, just coding methods. IMHO

[David Conigliaro CNC Software Inc.]

Let's stay out of the weeds relatoive to the whole Surfcam patent issue. CNC worked out a very stable and reliable approach to the code behind our Dynamic Mill motion...and we did our own way, it is all Mastercam!

[neil qwerty]

quote:

---

I've cleared P20 pockets with isalnds and such cutting 1 inch deep with a 1/2 inch cutter at over 700 IPM safely on Makino's and Okuma's.

---

Very interesting, what spindle speed and step over were you using to acomplish this?

[David Conigliaro CNC Software Inc.]

You cannot do this with just any carbide tool. I was using an Iscar CF series. You can safely run at 245IPM at 4584RPM, 489IPM at 9168RPM, 611IPM at 11,460RPM, or 733IPM at 13752RPM all at a 10% stepover. Yes it's a small stepover but the MRR is higher than traditional feeds and larger stepovers even if you choose to use RCTF for an adjustment. Technically you can go faster but will your machine achieve these high feedrates due to accel and decel? If you run these high feedrates on a machine that cannot achieve them due to weak acccel and decel, you will actually be running a much slower feedrate at the machine, which will generate much smaller chips that do not have the mass to pull heat away with them. That heat will then have to go some where like in the tool or the workpiece. You might want to choose the 244IPM for a slower machine. You have to know your equipment!

[Rob @ Target Machine]

Yeah. I'm jealous now. Those are some nice MRR's.

 

:going to the bank:

 

Penalty or not, I'm getting X4.

 

.

 

Dave - I'll stop beating on that blue horse.

[Roger Peterson]

Dave C. good to see you in on this topic!

 

The "issues" I've had with the cimco adaptive clearing in the past, which dynamic mill is very similar to, have to do with going around outside corners. While dynamic mill does a great job of keeping a consistent angle of engagement, that doesn't mean the tool load doesn't change.

 

Example: 45 degree engagement on a .5" endmill (.0732 stepover)

 

.200" move in straight line removes .0057 square inches of material

 

.200" moves where the direction of movement keeps at ~45 degrees that same .200" move removes .0329 square inches, 5 times more material is removed as it moves around an outside corner.

 

I know you don't have a 45 degree direction change consistantly over .200" but this is just an example to show how tool load changes.

 

Of course we can use the high feed filter to modify the feedrate based on volume, but if this could be incorporated directly into the dynamic mill that would save time and complexity.

 

 

HTH

[Rob @ Target Machine]

38 deg helix - variable pitch

 

Are those the CF series End Mills you used?

[David Conigliaro CNC Software Inc.]

They are a series of tools called CF. It stands for Chatter Free.

[Rob @ Target Machine]

I'll try em out. We have a bunch of Kovar to cut. That should be a good match for the tool.

[Michael Sullivan]

David,

 

do you think dynamic mill would be beneficial for this part:

 

http://www.emastercam.com/cgi-bin/ultimate...ic;f=1;t=034506

 

I tried to configure it,(as well as other paths) but couldn't get the path I wanted. I wanted to use trochoidal techniques because it is 304 stainless.

 

I could send you the file if you want to take a look.

 

Thanks,

 

-Mike

[David Conigliaro CNC Software Inc.]

Mike,

Send me the model if you have it or i can model somehting similar

[Michael Sullivan]

You've got mail David.

[Michael Sullivan]

That's exactly what I was looking for Dave.

 

I need training!

 

Dynamic Mill is the bomb!