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:

Boss Milling LOGO


tyler@goscpm.com
 Share

Recommended Posts

12 minutes ago, [email protected] said:

Can anyone help me generate some toolpaths to mill this logo? I keep getting errors... I just want the logo to be a .125 raised boss on top of this block. Ughhhh.

SCPM Logo THIS ONE.mcam

Well need to grab the right size tool. No way a 3/4 endmill is going to fit in that shape. I would use 3D Optirough on the solid and call it a day. That is too complex of a shape for 2D is going to be a fight and where 3D is the better choice IMHO. I went down to the 1/32 and got something to work. I am out of space on the forum to share screen shots and no time to go clean out old pictures. I went down to the 1/32 with a very small step over and 10% minimum toolpath radius and could machine the complete part. UNDER NO CIRCUMSTNACES TRY TO RUN THAT PROGRAM ON THE MACHINE!!!!  The problem is running too small of arc in HST toolpaths can ruin the linear bearings. 

Link to comment
Share on other sites

Just use a pocket toolpath and expand the outer chain that is around your part. Check your plane settings as well. I did a 1/8 cutter for the 1st toolpath and a remachining path with a 1/16 and it still didn't clean up. You need a smaller cutter like Ron suggested.

Personally I would have the top of the part at Z0, then all my moves in Z are - moves and easier to see in the code.

 

Pocket.JPG

  • Like 1
Link to comment
Share on other sites
1 hour ago, [email protected] said:

Are you saying not to run this file, though? 

Answer me this what is wrong with the file? I am not piking on you I want to use this as teaching process to help educate you and others to learn how to machine a part like this. 

I have 5 things I can think of right off the top of my head wrong with the file.

This is open to everyone. What have I done wrong?

 

Link to comment
Share on other sites

Crazy^millman shouldn't the machines controller Decelerate/accelerate where needed to prevent the machine from beating itself up, i am not sure if i am understanding what your saying correctly but I was under the impression the machine controller would slow it down to whatever feed the machine can actually handle. Like for example if I peel mill a little tiny slot, lets say .55" wide with a .5" tool so its swinging little arcs at 1000000ipm, my machine here will slow it down to whatever feedrate the machine can handle. I can throw a crazy feed at our haas super mini with next gen control and it will probably cut that peel mill a .55" wide slot with a .5" tool at like 50ipm even if i program it for 5000000ipm because the controller does its thing and decelerates to what its actually able to handle, it doesn't beat the crap out of the machine from my experience. and on other machines i have ran its been the same situation for me in the past so maybe you have seen that on a specific machine but i have not so i am not sure what you mean exactly. on top of that machines even have settings like haas's G187 settings that effect things like this. 


I am not saying that I typically like to peel mill/dynamic mill with that small of loops but nor do I ever throw a crazy feed like that into the program but just saying i have never seen the machine beat itself silly due to something like this so im having trouble imagining what your describing. 

 

Link to comment
Share on other sites
1 minute ago, JoshC said:

I am not saying that I typically like to peel mill/dynamic mill with that small of loops but nor do I ever throw a crazy feed like that into the program but just saying i have never seen the machine beat itself silly due to something like this so im having trouble imagining what your describing. 

If I understand what you're asking, it's about lubrication and wearing flat spots by the ball screw making many, many repeated small moves over the same area.

This type of cutting is well-known to cause those kinds of issues under those circumstances....maybe not this week...but done enough, eventually...

  • Like 1
Link to comment
Share on other sites
19 minutes ago, JParis said:

If I understand what you're asking, it's about lubrication and wearing flat spots by the ball screw making many, many repeated small moves over the same area.

This type of cutting is well-known to cause those kinds of issues under those circumstances....maybe not this week...but done enough, eventually...

well that makes sense then, I didn't think about that or never seen it happen either to me, my guess though is in order for that to happen it would have to be running the same cut day in and day out for years before it would actually happen in my opinion. probably wouldn't be much of a concern for me but I can see how some may worry about stuff like this. 

Link to comment
Share on other sites
18 minutes ago, JParis said:

If I understand what you're asking, it's about lubrication and wearing flat spots by the ball screw making many, many repeated small moves over the same area.

This type of cutting is well-known to cause those kinds of issues under those circumstances....maybe not this week...but done enough, eventually...

Yes sir that is the issue with running such small arcs pay me now or pay me later, but you will tear something up. The other issue was the LOC to ROC not going to happen. The RPM is not possible on most machine was the other error. I didn't define a holder to me a major error in today manufacturing, Our work as a programmers requires attention to detail and not defining a holder is an error in my humble opinion. The last error was the standard tool definition. It was wrong. I can think of not defining a stock model to start as something to help the process, but not required to start it. 

Rekd touched on the other issue I would problem use 3 tools to cut that shape. I would make progressive stock models after each tool and then do one last finish pass around the whole logo shape itself to make a nice looking part when I was done. Only way we can teach others is to have conversation like this. I hope Tyler and other have gained some knowledge and insight into this with this topic. 

Link to comment
Share on other sites
1 minute ago, JoshC said:

well that makes sense then, I didn't think about that or never seen it happen either to me, my guess though is in order for that to happen it would have to be running the same cut day in and day out for years before it would actually happen in my opinion. probably wouldn't be much of a concern for me but I can see how some may worry about stuff like this. 

We have to worry about stuff like this that is our job as programmers. I am called on to be the person in the know by a lot of companies and why I made the statement I did about not running the program the way I gave as the example. 

Just now, #Rekd™ said:

Not to mention small arcs can cause serious problems on older FANUC controls.....creating huge gouges. Vericut will give a warning on these. 

Another excellent point. 

  • Like 1
Link to comment
Share on other sites
7 minutes ago, crazy^millman said:

We have to worry about stuff like this that is our job as programmers. I am called on to be the person in the know by a lot of companies and why I made the statement I did about not running the program the way I gave as the example. 

Another excellent point. 

nah she will be fine, i'd let 'er rip, they make new ones every day ;)

but im the type of person that doesn't wear face masks driving down the highway so maybe im a rebel

  • Haha 1
Link to comment
Share on other sites
5 hours ago, JoshC said:

Crazy^millman shouldn't the machines controller Decelerate/accelerate where needed to prevent the machine from beating itself up, i am not sure if i am understanding what your saying correctly but I was under the impression the machine controller would slow it down to whatever feed the machine can actually handle. Like for example if I peel mill a little tiny slot, lets say .55" wide with a .5" tool so its swinging little arcs at 1000000ipm, my machine here will slow it down to whatever feedrate the machine can handle. I can throw a crazy feed at our haas super mini with next gen control and it will probably cut that peel mill a .55" wide slot with a .5" tool at like 50ipm even if i program it for 5000000ipm because the controller does its thing and decelerates to what its actually able to handle, it doesn't beat the crap out of the machine from my experience. and on other machines i have ran its been the same situation for me in the past so maybe you have seen that on a specific machine but i have not so i am not sure what you mean exactly. on top of that machines even have settings like haas's G187 settings that effect things like this. 


I am not saying that I typically like to peel mill/dynamic mill with that small of loops but nor do I ever throw a crazy feed like that into the program but just saying i have never seen the machine beat itself silly due to something like this so im having trouble imagining what your describing. 

 

5 hours ago, JoshC said:

Josh, It seems like there has been a lot of miss conception when it comes to dynamic milling.  First of all: I would say: unless you are milling 2.5D, it might not be worth it. Secondly, most modern machines have glass scales on encoders and memory buffers are capable of handling 2000 imp.

Yeah, I have read a lot about the wear on the ball screws due to minor movements. In fact I can attest to this. I do see  0.0005" back lash on a 63" table over period of 30 years.(most of it due to dropping the parts or hitting it with the fork lift!)

Mastercam has a setting to Decelerate in the corners. Same as a high speed toolpath option. None of it worked as intended!

 

Link to comment
Share on other sites

my point was just that running a dynamic path in a tight area is not going to ruin your machine if you do that occasionally, running a narrow peel mill type toolpath is not ideal in many circumstances but its not going to blow the machine up if you do it occasionally is all I was getting at with the way an earlier post kind of came off.

Link to comment
Share on other sites

we all think that 1 little slot will not wreck our 300k machine. But it could. i ran a matsura a few years ago. I had 1 slot to cut. 0.295 wide. 0.250 deep. Boss said use a 1/4" em. Ok. So programmed it 12k rpm 50ipm. Nice peel mill program. Slot was only 30 inch long. After i was done the machine was not sounding right. Felt rough in 1 spot on the table. Pulled covers off and had a look. Ball screw was pooched. linear bearings had a nice wear spot on them. about .005 play on the table right there. Called matsura to come fix it. They looked at it and right away asked what i cut with it right there. They knew exactly what happened. Too long moving just a few thou in same spot. They covered it under waranty but told boss not to do it again. So from then on i programmed allot differently. When i do long slots like that i break it up into short sections and come out of the cut above the part and run the table around just to lube bearing and cool them off. Then back into the cut. Bearings have been good for over 7yrs no problems.

Your mileage may vary but i dont suggest it.

 

  • Like 1
Link to comment
Share on other sites
On 10/10/2020 at 7:39 PM, JoshC said:

my point was just that running a dynamic path in a tight area is not going to ruin your machine if you do that occasionally, running a narrow peel mill type toolpath is not ideal in many circumstances but its not going to blow the machine up if you do it occasionally is all I was getting at with the way an earlier post kind of came off.

This has been documented a number of times and depends on the machine maker. If your machine lube is driven by the distanced moved rather than time you could be in trouble in relatively short order. Some machine sellers have refused (or put up a fight) to fix it under warranty.

  • Like 1
Link to comment
Share on other sites
24 minutes ago, Robert Ouellette said:

we all think that 1 little slot will not wreck our 300k machine. But it could. i ran a matsura a few years ago. I had 1 slot to cut. 0.295 wide. 0.250 deep. Boss said use a 1/4" em. Ok. So programmed it 12k rpm 50ipm. Nice peel mill program. Slot was only 30 inch long. After i was done the machine was not sounding right. Felt rough in 1 spot on the table. Pulled covers off and had a look. Ball screw was pooched. linear bearings had a nice wear spot on them. about .005 play on the table right there. Called matsura to come fix it. They looked at it and right away asked what i cut with it right there. They knew exactly what happened. Too long moving just a few thou in same spot. They covered it under waranty but told boss not to do it again. So from then on i programmed allot differently. When i do long slots like that i break it up into short sections and come out of the cut above the part and run the table around just to lube bearing and cool them off. Then back into the cut. Bearings have been good for over 7yrs no problems.

Your mileage may vary but i dont suggest it.

 

 

4 minutes ago, nickbe10 said:

This has been documented a number of times and depends on the machine maker. If your machine lube is driven by the distanced moved rather than time you could be in trouble in relatively short order. Some machine sellers have refused (or put up a fight) to fix it under warranty.

Exactly what I have seen on other machines why said it was an example only.

  • Like 1
Link to comment
Share on other sites

It's all about whether the move exceeds the bearing spacing or not.  If not, it can push all the lube out of the way and have dry metal-on-metal rolling, causing false brinelling.  I learned about this the hard way cutting .020" wide slots with a .010" endmill.  12 slots per part (indexed on a rotary so they're all in the exact same Y position), 1/2" long each, 12 parts, ruined my thrust bearings on the Y axis.  Got them replaced, then next time I had to make the parts I'd cut a third of a slot, pick up, move 3" diagonal and back, then cut another third, etc.  No damage since.

So in my opinion, if you're dynamic milling around a part in different places, you should be fine.  It's the long narrow slots along one axis that'll kill it.

  • Like 1
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...