Leon82

Feed mills and optirough

Recommended Posts

Does mastercam comp the optirough to feed mills if you use custom geometry?.

Share this post


Link to post
Share on other sites

That's been a question of mine for ages.  I'm curious to see what response you get.  We suggest defining them as a bull mill using the "programming" radius in the book for our tools.  I have never felt comfortable with that though.  I have always been curious.  Me personally I have used a custom definition 99% of the time.  But I don't recall if I was using optirough or not.  I do know that using the custom definition, stock models and verify take way too much horsepower to calculate in comparison to using a bull mill or stock feedmill definition.

At the end of the day, as long as your tool definition creates an extra stock on condition, and your stepover doesn't create islands which overrun your depth of cut capability.  It shouldn't matter much.  You aren't using feed mills for anything other than roughing right?  Chances are you need to go do some rest roughing anyway.  That said, it would be nice for the rest roughing stock to be 100% accurate within the stl creation tolerance and not have extra stock in places you don't expect it due to using a slightly different definition.

  • Like 1

Share this post


Link to post
Share on other sites
8 minutes ago, huskermcdoogle said:

That's been a question of mine for ages.  I'm curious to see what response you get.  We suggest defining them as a bull mill using the "programming" radius in the book for our tools.  I have never felt comfortable with that though.  I have always been curious.  Me personally I have used a custom definition 99% of the time.  But I don't recall if I was using optirough or not.  I do know that using the custom definition, stock models and verify take way too much horsepower to calculate in comparison to using a bull mill or stock feedmill definition.

At the end of the day, as long as your tool definition creates an extra stock on condition, and your stepover doesn't create islands which overrun your depth of cut capability.  It shouldn't matter much.  You aren't using feed mills for anything other than roughing right?  Chances are you need to go do some rest roughing anyway.  That said, it would be nice for the rest roughing stock to be 100% accurate within the stl creation tolerance and not have extra stock in places you don't expect it due to using a slightly different definition.

yea, I usually kept it far away then rest machines with a bull insert mill

Share this post


Link to post
Share on other sites

I learned a new approach from Ron recently, which I really like.

  1. Create an Opti-Rough with Solid Carbide Endmills. No step-ups allowed. Force the Operation to use only "full flute depths of cut". (Ok, like 90-95% of the LOC.)
  2. Now perform an Opti-Rest with your Feed Mill. Define it as a Bull, so the calculations are quicker, and don't exceed the "max DOC" of the tool. This will do a "waterfall approach" (waterline), where you're just rest-roughing from the top-down, and you don't have any islands left-over from the previous roughing, because you weren't using your Feed Mill to rough away the bulk of the material.
  • Like 2

Share this post


Link to post
Share on other sites
2 minutes ago, Colin Gilchrist said:

I learned a new approach from Ron recently, which I really like.

  1. Create an Opti-Rough with Solid Carbide Endmills. No step-ups allowed. Force the Operation to use only "full flute depths of cut". (Ok, like 90-95% of the LOC.)
  2. Now perform an Opti-Rest with your Feed Mill. Define it as a Bull, so the calculations are quicker, and don't exceed the "max DOC" of the tool. This will do a "waterfall approach" (waterline), where you're just rest-roughing from the top-down, and you don't have any islands left-over from the previous roughing, because you weren't using your Feed Mill to rough away the bulk of the material.

That would be a lot of carbide endmills. I need to remove about 100 pounds

Share this post


Link to post
Share on other sites
1 minute ago, Leon82 said:

That would be a lot of carbide endmills. I need to remove about 100 pounds

What's the material?  I don't think you would need as many tools as you think, unless you are cutting something reallllly crappy.

But yes tool cost per cube removed is very good with feedmills typically, and in the many applications can go toe to toe on time with solids.

I like the concept of Ron's that Colin mentioned.  Has many merits.  Mainly that you maintain a high level of MRR while using the solid carbide tool, and don't wear it out or have poor cutting conditions due to stepping up and not utilizing the entire flute length.  The rest roughing using the feedmill will be a little slow MRR wise, but will be very cost effective and super high level of process security regardless if it is a solid feedmill or inserted.  Using solid feedmills would then give you very favorable l/d ratios to reach pretty deep with small diameter cutters that normal endmills might complain doing.

  • Like 1

Share this post


Link to post
Share on other sites
2 minutes ago, huskermcdoogle said:

What's the material?  I don't think you would need as many tools as you think, unless you are cutting something reallllly crappy.

But yes tool cost per cube removed is very good with feedmills typically, and in the many applications can go toe to toe on time with solids.

I like the concept of Ron's that Colin mentioned.  Has many merits.  Mainly that you maintain a high level of MRR while using the solid carbide tool, and don't wear it out or have poor cutting conditions due to stepping up and not utilizing the entire flute length.  The rest roughing using the feedmill will be a little slow MRR wise, but will be very cost effective and super high level of process security regardless if it is a solid feedmill or inserted.  Using solid feedmills would then give you very favorable l/d ratios to reach pretty deep with small diameter cutters that normal endmills might complain doing.

Commercially Pure titanium grade 2

 

It's round bar horizontal also so I need to start with the crest

Share this post


Link to post
Share on other sites

Yeah feedmill will be more efficient in that case. 

Per my maths...  I figure with full depth of cut with a 6 flute 1/2 x 1.5 tool, you could get about .85lb/min of material removal.  FWIW, IF, you could go full depth the whole time, I'd figure on about 2 endmills to get the job done.  But given working up to the crest it won't be that nice and you would end up wearing off the end of the tool before wearing out the rest of the tool.   Soo.... yeah.

Not that you had asked what the best way to do this was, but. Maybe post a dummy file and see if the collective brain trust has some goodness to offer that hadn't/hasn't been considered.

Maybe a hybrid stepped approach?  Work it with a feedmill until you could get some good solid full depth steps you could remove with solid tools  Not knowing the geometry of what you are doing makes this a fun guessing game.  Could be way off base on that approach.

Share this post


Link to post
Share on other sites

Colin there you go giving away all my secrets.  🤣 J/K

Yes I have seen the exact opposite happen with this approach. I let the solid carbide do the roughing and the MMR is impressive and the tools wear so much better than the traditional Step down to Up process currently promoted. Problem with the step up process is the tool starts getting uneven wear on the flutes and not even wear that full depths are doing. By keeping the solid carbide doing what it should be doing for the roughing you extend its tool life depending on the part 5-10 fold verse stepping up. Now the High feed cutter is the other part of the process using it at it strength for what it does. Put a Tool Inspection in thew program and then as you start cutting you have the disposable tool doing what it should be doing. I asked CNC software for this ability in OPTI-ROUGH some years ago, but still don't see it in the next BETA cycle. This does require a Stock model after you have used the Solid Carbide endmill, but try this process hard metals or gummy metals as in this case has been good where I have used it. The High-feed can have High Positive inserts purchased for it to help on the gummy material.

Husker Yes depending on the part you may have to do a Solid Carbide Endmill step then high-feed then do the next Solid Carbide Endmill step and then a high-feed.

In the case of this [part starting with Round stock I am thinking may not be needed, but again sight unseen hard to know.

  • Like 2

Share this post


Link to post
Share on other sites
On 1/14/2022 at 11:44 AM, crazy^millman said:

Colin there you go giving away all my secrets.  🤣 J/K

Yes I have seen the exact opposite happen with this approach. I let the solid carbide do the roughing and the MMR is impressive and the tools wear so much better than the traditional Step down to Up process currently promoted. Problem with the step up process is the tool starts getting uneven wear on the flutes and not even wear that full depths are doing. By keeping the solid carbide doing what it should be doing for the roughing you extend its tool life depending on the part 5-10 fold verse stepping up. Now the High feed cutter is the other part of the process using it at it strength for what it does. Put a Tool Inspection in thew program and then as you start cutting you have the disposable tool doing what it should be doing. I asked CNC software for this ability in OPTI-ROUGH some years ago, but still don't see it in the next BETA cycle. This does require a Stock model after you have used the Solid Carbide endmill, but try this process hard metals or gummy metals as in this case has been good where I have used it. The High-feed can have High Positive inserts purchased for it to help on the gummy material.

Husker Yes depending on the part you may have to do a Solid Carbide Endmill step then high-feed then do the next Solid Carbide Endmill step and then a high-feed.

In the case of this [part starting with Round stock I am thinking may not be needed, but again sight unseen hard to know.

Ron, do you have an example of the process Colin described that you could upload?

Share this post


Link to post
Share on other sites
4 minutes ago, JB7280 said:

Ron, do you have an example of the process Colin described that you could upload?

Sorry I cannot share that work it is under NDA.

  • Like 1

Share this post


Link to post
Share on other sites
6 minutes ago, crazy^millman said:

Sorry I cannot share that work it is under NDA.

No problem.  I'm having a little bit of difficulty understanding the process.  Or perhaps just understanding the purpose, or intention of the process.  Is the purpose to prevent an endmill with, say 50mm flute length, from taking cuts where it only engages say, 5mm of the flute, or whatever the step up is set to?  And using the feed mill, (which is meant to take smaller DOC) to machine those step-ups?

Share this post


Link to post
Share on other sites
3 hours ago, JB7280 said:

No problem.  I'm having a little bit of difficulty understanding the process.  Or perhaps just understanding the purpose, or intention of the process.  Is the purpose to prevent an endmill with, say 50mm flute length, from taking cuts where it only engages say, 5mm of the flute, or whatever the step up is set to?  And using the feed mill, (which is meant to take smaller DOC) to machine those step-ups?

That is exactly it. The problem with the step up process is the wear on the endmill in hard metals is not the full length of the endmill. The Carbide endmill for Opti-Rough in hard metals preforms at it's best when taken a full cut. Any Step up starts adding wear to that part of the flute. We are always trying to balance cut time to cost in anything we do. Running one off parts who cares get it done, but when you start looking at 20-50-100 or even 1000 parts even the smallest change can have a big impact on the ROI. We have to spend money to make money bottom line. The thought is why spend more money than we need if the process supports the best metal removal at the best price. Solid Carbide Endmills are expensive and we end up throwing away a good chuck of carbide in the shank. Head style tools are my biggest price break change on long running projects. The other is highfeed tools doing the step down process flipping the whole Opti-Rough on it's head. Still use OPTI-Rough to get big chucks of metal off the part, but start stepping down in full cuts with the solid Carbide then stepping down with high feed that are .02" per tooth on 4-10 flute tools getting in all reality a better detail in most cases than the stepping up was getting. Again only in hard to machine materials do I go this route, but in Softer materials where the endmill doesn't wear stepping up is just fine. The harder metals wear tools plain and simple and the idea is to let the wear work where it needs to work on the tools designed to wear how they were designed to wear. High Feed Cutters are made to take shallow cuts at high feeds not standard carbide endmills we use for Opti-Rough Toolpaths.

  • Like 1

Share this post


Link to post
Share on other sites
1 hour ago, crazy^millman said:

That is exactly it. The problem with the step up process is the wear on the endmill in hard metals is not the full length of the endmill. The Carbide endmill for Opti-Rough in hard metals preforms at it's best when taken a full cut. Any Step up starts adding wear to that part of the flute. We are always trying to balance cut time to cost in anything we do. Running one off parts who care get it done, but when you start looking at 20-50-100 or even 1000 parts even the smallest change can have a big impact on the ROI. We have to spend money to make money bottom line. The thought is why spend more money than we need if the process supports the best metal removal at the best price. Solid Carbide Endmills are expensive and we end up throw away a good chuck of carbide in the shank. Head style tools are my biggest price break change on long running projects. The other is highfeed tools doing the step down process flipping the whole Opti-Rough on it's head. Still use OPTI-Rough to get big chucks of metal off the part, but start stepping down in full cuts with the solid Carbide then stepping down with feed that are .02 per tooth on 4-10 flute tools getting in all reality a better detail in most cases than the stepping up was getting. Again only in hard to machine materials do I go this route, but in Softer materials where the endmill doesn't wear stepping up is just fine. The harder metals wear tool plain and simple and the idea is to let the wear work where it needs to work on the tools designed to wear how they were designed to wear. High Feed Cutters are made to take shallow cuts at high feed not standard carbide endmills we use for Opti-Rough Toolpaths.

Do you find you're able to get close to the MRR of high-feed mills, with solid carbide?  My feed mill toolpaths have always had a much higher MRR than my solid carbide toolpaths, but that could very well be because I'm just not pushing those endmills hard enough.

Share this post


Link to post
Share on other sites
12 minutes ago, JB7280 said:

Do you find you're able to get close to the MRR of high-feed mills, with solid carbide?  My feed mill toolpaths have always had a much higher MRR than my solid carbide toolpaths, but that could very well be because I'm just not pushing those endmills hard enough.

MMR with Solid Carbide in Hard Metals verses High Feed just don't match up. Run time is the difference though it would always seem that shouldn't be the case. The difference is how much time does the machine stop to change the inserts on the high feed cutters verses Solid Carbide endmillls? Now if I have 4 of the same tool in the machine using a parent child process where the machine was never stopped to replace the inserts then we slide the run time back to the High-Feed Cutter, but how many shops are doing roughing this way? MMR is important don't get me wrong, but I can think of a situation where Ceramic can remove tons of Inconel, but after 4-5 minutes that tool has to be replaced. Now a Carbide tool can cut for 2 hours unattended and not super heat the metal removing the material like the Ceramic tool does. About the same amount of MMR, but one took 4 minutes and one took 2 hours. One is constantly replacing really expensive tools and one is replace less expensive tools, but is more predicable in the process. Which one do you want to use as your process? That is kind of the idea here. Which one is more predicable and removes the material with the less amount of interruptions?

Share this post


Link to post
Share on other sites
17 hours ago, crazy^millman said:

MMR with Solid Carbide in Hard Metals verses High Feed just don't match up. Run time is the difference though it would always seem that shouldn't be the case. The difference is how much time does the machine stop to change the inserts on the high feed cutters verses Solid Carbide endmillls? Now if I have 4 of the same tool in the machine using a parent child process where the machine was never stopped to replace the inserts then we slide the run time back to the High-Feed Cutter, but how many shops are doing roughing this way? MMR is important don't get me wrong, but I can think of a situation where Ceramic can remove tons of Inconel, but after 4-5 minutes that tool has to be replaced. Now a Carbide tool can cut for 2 hours unattended and not super heat the metal removing the material like the Ceramic tool does. About the same amount of MMR, but one took 4 minutes and one took 2 hours. One is constantly replacing really expensive tools and one is replace less expensive tools, but is more predicable in the process. Which one do you want to use as your process? That is kind of the idea here. Which one is more predicable and removes the material with the less amount of interruptions?

Thank you Ron.  The effort you seem to put into every reply is ALWAYS greatly appreciated!!

Share this post


Link to post
Share on other sites
2 hours ago, JB7280 said:

Thank you Ron.  The effort you seem to put into every reply is ALWAYS greatly appreciated!!

Had a boss said I talked to much and put to much in my email responses. Short and sweet sometimes just don't cut it.

  • Like 1

Share this post


Link to post
Share on other sites

its going to backfeed over a rib left because the programing radius is less than the cutting radius. I'm going to have to adjust my plan

Share this post


Link to post
Share on other sites

in verify it seems to clean up the rib with a custom profile for a feedmill type tool

Share this post


Link to post
Share on other sites
14 minutes ago, Leon82 said:

its going to backfeed over a rib left because the programing radius is less than the cutting radius. I'm going to have to adjust my plan

Change your retract settings where needed to have it move out of the areas verses doing a back feed operations.

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • 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