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:

Are their any downsides to Dynamic Milling?


monkeyman
 Share

Recommended Posts

1 hour ago, cncappsjames said:

Two CAD/CAM/CAE/PLM companies shovel this kind of bullshiite; Siemens and Dassault (CATIA). Why? Because their CAM product is inferior to probably half a dozen CAM packages out there and they are embarassed about it. So, they peddle lies to their customers in hopes their inferiority won't be exposed. Their CAD/CAE/PLM packages are excellent however... CAM... not so much.

Yes sat in many meetings with different customers using both. I had one owner point blank ask me why do I program in Mastercam and not CATIA. I said Mastercam can do everything I need it to do. CATIA and NX both have to use Voluemill to match Mastercam for Dynamic milling. Plus why would I spend 4X the money on a seat of software? I am a smarter business man that that.

  • Like 4
Link to comment
Share on other sites
18 hours ago, cncappsjames said:

Two CAD/CAM/CAE/PLM companies shovel this kind of bullshiite; Siemens and Dassault (CATIA). Why? Because their CAM product is inferior to probably half a dozen CAM packages out there and they are embarassed about it. So, they peddle lies to their customers in hopes their inferiority won't be exposed. Their CAD/CAE/PLM packages are excellent however... CAM... not so much.

I agree that the CAD/CAE/PLM side of NX and Catia are good products for design and engineering verification. However, a friend calls the CAM side of these brands: "Afterthought engineering".    CAM was not their primary focus.

 

One of the things that I have experienced over the years is: Tier 1 manufacturering managment buying into the sales pitch that "The engineer will make a design change and everything downstream will be automatically updated.  The programmer won't even have to look at, or have make any changes to the program, it will be automatic."  A recipe for disaster.

 

 

  • Like 3
Link to comment
Share on other sites

NX and CATIA CAM as an afterthought.... yeah. That is SPOT on. Their power isn't in the the quality of their metal removal processes contrary to their sales slime lies, their power is in their integration with Engineering. But like what Bill said, that sounds good on paper, but in real life can be disastrous if the Engineer and Programmer are not the same person. 

Link to comment
Share on other sites

Dynamic milling gets a lot of praise and it deserves it, but I feel like playing devils advocate here and offer some words of caution. Some people I work with have fallen into the trap that dynamic is the be all end all of roughing.  They program their toolpaths to be too "dynamic".  By that I mean that they think that they can just put the stepover really light and the feedrate really high and get the same or faster cycle time. But in reality the main downfall for dynamic milling are the linking moves and the capability of the machine to accel/decel.  A decreasing your stepover percentage means you are increasing your linking moves by the same percentage which to me is wasted machine motion. And this becomes worse if the feature you are cutting is a closed pocket. There is a very high chance that your machine won't even hit your programmed feed rate, let alone maintain it. This can have an exponential effect on your actual cycle time. Sometimes it is better to just slow down and increase your stepover.

Just my observations based on my current place of work and something I am trying to get people away from. As someone else said, programming is a series of trade offs. Sometimes it can be more efficient to throw a quick optirough on a one off part and let the machine work. If a part is going to be a repeat one, then it is time to sit down and work through some cycle time analysis and explore options other than dynamic.

  • Like 2
Link to comment
Share on other sites
20 hours ago, cncappsjames said:

 but in real life can be disastrous if the Engineer and Programmer are not the same person. 

Very rigid and defined processes are needed to make this work, even then it still falls short.  We have had some projects recently that have tried to capture this capability for some product families, it's now better than it was but it is very custom.  This is in NX.

Link to comment
Share on other sites
2 hours ago, rgrin said:

If a part is going to be a repeat one, then it is time to sit down and work through some cycle time analysis and explore options other than dynamic.

Almost always, if the geometry has any complicated features, or if it is 3d roughing, Dynamic or Opti is going to be better.  The biggest decision that needs to be made will usually be in what to use for a stepover.  Sometimes, a 40-60% or even greater in shallow applications stepover with dynamic motion with conventional speeds and feeds will yield very very good predictable results and will yield more productivity in tool life and process reliability than a conventional toolpath, with only a small cycle time premium.  On paper the MRR might be more with a light stepover with speed bonus, but the extra air cutting and acc/dec slowdowns make it overall slower.  Heavy radial stepovers make for a good balance without a lot of extra air cutting.

  • Like 3
Link to comment
Share on other sites
2 hours ago, huskermcdoogle said:

Sometimes, a 40-60% or even greater in shallow applications stepover with dynamic motion with conventional speeds and feeds will yield very very good predictable results and will yield more productivity in tool life and process reliability than a conventional toolpath, with only a small cycle time premium.

I use Optirough without stepups to program high feed cutters at 65% stepover.  Works a treat.

  • Like 3
Link to comment
Share on other sites
6 hours ago, rgrin said:

Dynamic milling gets a lot of praise and it deserves it, but I feel like playing devils advocate here and offer some words of caution. Some people I work with have fallen into the trap that dynamic is the be all end all of roughing.  They program their toolpaths to be too "dynamic".  By that I mean that they think that they can just put the stepover really light and the feedrate really high and get the same or faster cycle time. But in reality the main downfall for dynamic milling are the linking moves and the capability of the machine to accel/decel.  A decreasing your stepover percentage means you are increasing your linking moves by the same percentage which to me is wasted machine motion. And this becomes worse if the feature you are cutting is a closed pocket. There is a very high chance that your machine won't even hit your programmed feed rate, let alone maintain it. This can have an exponential effect on your actual cycle time. Sometimes it is better to just slow down and increase your stepover.

Just my observations based on my current place of work and something I am trying to get people away from. As someone else said, programming is a series of trade offs. Sometimes it can be more efficient to throw a quick optirough on a one off part and let the machine work. If a part is going to be a repeat one, then it is time to sit down and work through some cycle time analysis and explore options other than dynamic.

Most people I have come across don't really know how maximize dynamic tool paths.  They don't understand that, depending on material and tooling, you can go full depth of cut.  They also make the mistake of going to light on the radial depth of cut.  Also, they don't filter their programs, so the go to the machine and it looks too slow.  IF you use the filters its going to be much faster.

Link to comment
Share on other sites
19 minutes ago, AMCNitro said:

Most people I have come across don't really know how maximize dynamic tool paths.  They don't understand that, depending on material and tooling, you can go full depth of cut.  They also make the mistake of going to light on the radial depth of cut.  Also, they don't filter their programs, so the go to the machine and it looks too slow.  IF you use the filters its going to be much faster.

Also, I highly encourage anyone running these to figure out what the maximum speed your particular machine can run through X radius (Cut Parameters > Minimum toolpath radius).  For example, on a lighter weight linear rail machine, it may be able to sustain 400 IPM through a .2", but your older, belt driven box-way machine would be lucky to reach 120.   So if you're programming for the linear rail machine, plan on getting better cut times by really ramping up the feed and lowering the stepover, but with the box way machine you have to lean towards heavier cuts slower.

And of course, remember to use your "back feed rate" to the max rate of the machine & control can manage to limit that air cutting time. 

  • Thanks 1
  • Like 1
Link to comment
Share on other sites

Yea, sometimes you can use pocket with high speed roughing pattern and do the .5x down .5x over and really rip it out in aluminum. But you need the horsepower to avoid alarms.  dynamic uses less horsepower and can keep the flute wear more even. 

Link to comment
Share on other sites
On 5/20/2022 at 2:49 PM, crazy^millman said:

He didn't know how to program the machines I was in there working on. He knew 5 Axis programming, but not Mill/Turn. I was using an inferior software to program with in his mind. He is a NX snob and me using Mastercam makes me a second rate programmer. Funny the head of Purchasing had instructed the purchasing department to not send 5 Axis work to shop using Mastercam. When he found out our group was using Mastercam to program their parts and heard what we were doing he called me and I told him yes the rumor is true Mastercam can program any machine you have. They changed their policy after that conversation.

The problem as I see it, is that Mastercam is somewhat intuitive if you are a machinist.  Because a skilled machinist can jump on it with a very short lesson and get some use out of it, management seems to be reluctant to pay for training (in my experience).  So on the marketing end, Mastercam is undersold.  However, I bet nobody at CNC Software would say with a straight face to a perspective customer, "we have the FANUC kernel embedded in out software, so you will get perfect code every time".  That statement, from brand x CAM company, even got me for about 5 seconds.  Wait a minute, how does having the kernel in your software know how all the parameters on our machine are set up?  Two same exact model machines can be set up differently...  I have been told what Mastercam "can't" handle, but never had a show stopper that a little post magic or lying on a tool definition etc couldn't cure.  Other softwares, if it can't do it, usually means you can't either.

Link to comment
Share on other sites
30 minutes ago, bd41612 said:

we have the FANUC kernel embedded in out software, so you will get perfect code every time

I remember when I saw that... I about died laughing. We need to make THAT guy famous.

32 minutes ago, bd41612 said:

Wait a minute, how does having the kernel in your software know how all the parameters on our machine are set up?  Two same exact model machines can be set up differently... 

Exactly right. Also, let's say a Brand X machine comes from the factory with a suite of options. Serial number 12345. Chances are things will at least work. Maybe the parameters need some massaging, but no alarms when you activate something. Now, take same Brand X machine serial number 12346 leaves the factory without said suite of options... then FANUC comes and installs the options. Chances are the field service tech isn't going to know everything to get those options going and here the ride begins...

"FANUC Kernel"

RFLMFAO

Link to comment
Share on other sites
6 hours ago, huskermcdoogle said:

Sometimes, a 40-60% or even greater in shallow applications stepover with dynamic motion with conventional speeds and feeds will yield very very good predictable results and will yield more productivity in tool life and process reliability than a conventional toolpath

I was involved runnig some tests on a VF5 50 taper mill for Dynamic toolpath power cuts with a 10mm end mill with 75% stepover at 2 times diameter deep in 4140 and 304 stainless. 

It was amazing to watch.  We were drawing 80% load on a 50 taper spindle with a .39 diameter end mill.   The cycle time was shorter and the file size and lookkahead were more friendly.

Here is a link to a Cimquest video showing the difference.

https://www.youtube.com/watch?v=Bi2j-Q-G0sM

 

 

 

Edited by Bill Craven
edited for clarity
  • Like 2
Link to comment
Share on other sites
9 hours ago, Aaron Eberhard said:

And of course, remember to use your "back feed rate" to the max rate of the machine & control can manage to limit that air cutting time. 

And don't forget to optimize your gap size distance; sometimes it's faster to retract and rapid than to backfeed, especially if it's going to the other side of the part.

  • Like 1
Link to comment
Share on other sites

If there is any downside to dynamic milling is it can create the misconception that it needs to be used everywhere. I have seen guys program a .560 wide slot using a 1/2" endmill. Yes it can make the part, but that short motion is not good on machines & takes longer than just going old school and cutting a slot. I have seen others dynamic mill a keyway in a mild steel shaft.

 

  • Like 3
Link to comment
Share on other sites
1 hour ago, MIL-TFP-41 said:

I have seen guys program a .560 wide slot using a 1/2" endmill. Yes it can make the part, but that short motion is not good on machines

Yes... I have seen a Y axis lead screw get a bad spot worn in it by a toolpath like this in a production environment

 

  • Like 3
Link to comment
Share on other sites
6 hours ago, bd41612 said:

So you know who I'm talking about?

Actually I do not know who the sales guy that said that is. I just recall the conversation here somewhere (perhaps it was in the old OT Forum)... I can't seem to locate it. But "FANUC kernel" is what I remember... as if there's such a thing... ROFLMFAO. That is worthy to make fun of because it was said with such authority.

Link to comment
Share on other sites
6 hours ago, MIL-TFP-41 said:

If there is any downside to dynamic milling is it can create the misconception that it needs to be used everywhere. I have seen guys program a .560 wide slot using a 1/2" endmill. Yes it can make the part, but that short motion is not good on machines & takes longer than just going old school and cutting a slot. I have seen others dynamic mill a keyway in a mild steel shaft.

 

This can also damage your thrust bearings through fretting, if the reciprocal motion is smaller than the bearing spacing.

  • Like 3
Link to comment
Share on other sites
On 5/23/2022 at 4:26 PM, Aaron Eberhard said:

And of course, remember to use your "back feed rate" to the max rate of the machine & control can manage to limit that air cutting time. 

A Matsuura H.Plus-500 that I often program for has a "max feedrate" equal to it's rapid feed, which I believe is 2800ipm.  I usually set my back feedrate to 1200.  I just can't fathom it moving at 2800ipm without clipping corners, even with look-ahead turned on.  I supposed I should test it out one of these days.  

  • Like 2
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...