Facing Round Parts in CNC Mill - Rework

zipfactor · May 13, 2017

Preface: I am a CNC newbie. I know enough to be dangerous, etc....

I ran a batch of 25 parts and goofed up the finished thickness. Apparently the hard stop on my bandsaw cutting the blanks moved a bit, throwing off the starting stock dimensions. Anyhow....

I'd like to rework these discs for the correct thickness. I have a set of soft jaws on the vise which locates the part roughly the same height every time from the vise body. As the thickness of the parts vary, I would like to set up a program that starts at a height just above the thickest measured part in the lot, and faces off to a set height. Conceptually, I'm not sure how to set up a program to due what I am suggesting. I use HSMWorks with Solidworks for CAD/CAM.

Any advice would be helpful, as I'm honestly not sure where to start. Thanks guys.

Limy Sami · May 13, 2017

Your ''I have a set of soft jaws on the vise which locates the part roughly the same height every time from the vise body'' (my bold italics) Is just asking for trouble,

Find a way - like setting the parts on parallels of getting a proper datum to work from BEFORE you start worrying about progamming etc etc etc

zipfactor · May 13, 2017

Limy Sami said:
Your ''I have a set of soft jaws on the vise which locates the part roughly the same height every time from the vise body'' (my bold italics) Is just asking for trouble,

Find a way - like setting the parts on parallels of getting a proper datum to work from BEFORE you start worrying about progamming etc etc etc

Roughly in this sense is repeatable within 0.25mm in the z direction. Close enough for the job.

litlerob1 · May 13, 2017

Well you don't need Solidworks for this, holy shit. In HSM works create a circle, translate it above Z zero by the thickness of the finished part. Then toolpath from there, Jockey.

R

zipfactor · May 13, 2017

litlerob1 said:
Well you don't need Solidworks for this, holy shit. In HSM works create a circle, translate it above Z zero by the thickness of the finished part. Then toolpath from there, Jockey.

R

No denying the jockey title

.

The part was already modeled in solidworks. I wanted to give the complete picture.

carbonbl · May 13, 2017

Within the HSMWorks facing toolpath, set your "Top" height at the height of the thickest piece of stock above your Z datum. You can set this off some feature in solidworks or just a measurement above Z. Setting it slightly higher may be advisible depending on cutting conditions and repeatability of your fixture. Set the "Bottom" to whatever you want the final face depth to be. In the next tab, check multiple depths and choose a reasonable "maximum roughing stepdown" for your cutting conditions (tool, material, machine etc). Specify a finishing step if you want. As long as your WCS, tool offset and other basic things are set correctly, this will generate a toolpath that will step down multiple depths to your final facing depth. Of course, the thinner parts will have some air cutting before the tool contacts them.

zipfactor · May 13, 2017

carbonbl said:
Within the HSMWorks facing toolpath, set your "Top" height at the height of the thickest piece of stock above your Z datum. You can set this off some feature in solidworks or just a measurement above Z. Setting it slightly higher may be advisible depending on cutting conditions and repeatability of your fixture. Set the "Bottom" to whatever you want the final face depth to be. In the next tab, check multiple depths and choose a reasonable "maximum roughing stepdown" for your cutting conditions (tool, material, machine etc). Specify a finishing step if you want. As long as your WCS, tool offset and other basic things are set correctly, this will generate a toolpath that will step down multiple depths to your final facing depth. Of course, the thinner parts will have some air cutting before the tool contacts them.

Thank you, exactly what I was thinking but hadnt a chance to muck with it yet.

Ridethelighting · May 13, 2017

I can't see where cad/cam is needed. Write a quick g code program and make chips. By time you open the whatever program and draw a circle you should be making at least the first depth cut.

Hazzert · May 13, 2017

Ridethelighting said:
I can't see where cad/cam is needed. Write a quick g code program and make chips. By time you open the whatever program and draw a circle you should be making at least the first depth cut.

Agreed, I would be Zeroing my home position at finished thickness and just work down on all these parts until you get to zero.

litlerob1 · May 14, 2017

Here's a thought, 25 parts? Put them in that other machine that spins the part instead of the tool, and face them that way. You woulda been done about an hour after you started this thread. Or if you NEED to use a Milling machine, there should be a hand wheel, or a jog function??

R

Captdave · May 15, 2017

We cut a ton of 6" and 5.25" and several other sizes 6061 Rod and all the drops go into bins according to diameter to be sorted out later. Once sorted by thickness then we put them on a mill with 5 double vises and get after them with a 1/2" EM with a circular HSM tool path with a reasonable stepover, who cares if the removal amount is .100" or 1.0" and go do something else for 8 minutes. Try that on your lathe.....once

gorrilla · May 15, 2017

Captdave said:
We cut a ton of 6" and 5.25" and several other sizes 6061 Rod and all the drops go into bins according to diameter to be sorted out later. Once sorted by thickness then we put them on a mill with 5 double vises and get after them with a 1/2" EM with a circular HSM tool path with a reasonable stepover, who cares if the removal amount is .100" or 1.0" and go do something else for 8 minutes. Try that on your lathe.....once

.100 or 1.00 removal amount with a 1/2 EM? Even with HSM that's a LOT of passes to get 1" of material removed. I understand you are loading 5 parts at once, but as a general rule, removing metal in a lathe is more efficient than in a mill. .100 is one thing, but 1.00! Another animal altogether. Add to that you are facing ROUND stock in a vise. If you have jaws made to grab the radius, you can get a lot more bite, but that's the only way you can compete. THe ability to load several parts at once WOULD be worth a lot, but 8 minutes removing 1" facing off 5 parts with helical interpolation on a mill with a half inch end mill? THAT would be impressive. But I'd have to see that.
The OP said nothing about what material he is cutting. Not everything in this world is aluminum. If he's cutting steel, of nearly any kind at all, you have to at least triple the time for aluminum. Some other stuff, even more. I wouldn't discount the idea of doing them in a lathe so quickly. Write a G72 facing program, starting at the longest part, add a reasonable depth of cut per pass, load a part, push the button, come back when she quits. Should be able to produce parts to the thou easily.
But like others here, I see no reason to have to use a program to write that program. I write them longhand every day, at the machine.

Captdave · May 15, 2017

gorrilla said:
.100 or 1.00 removal amount with a 1/2 EM? Even with HSM that's a LOT of passes to get 1" of material removed. I understand you are loading 5 parts at once, but as a general rule, removing metal in a lathe is more efficient than in a mill. .100 is one thing, but 1.00! Another animal altogether. Add to that you are facing ROUND stock in a vise. If you have jaws made to grab the radius, you can get a lot more bite, but that's the only way you can compete. THe ability to load several parts at once WOULD be worth a lot, but 8 minutes removing 1" facing off 5 parts with helical interpolation on a mill with a half inch end mill? THAT would be impressive. But I'd have to see that.
The OP said nothing about what material he is cutting. Not everything in this world is aluminum. If he's cutting steel, of nearly any kind at all, you have to at least triple the time for aluminum. Some other stuff, even more. I wouldn't discount the idea of doing them in a lathe so quickly. Write a G72 facing program, starting at the longest part, add a reasonable depth of cut per pass, load a part, push the button, come back when she quits. Should be able to produce parts to the thou easily.
But like others here, I see no reason to have to use a program to write that program. I write them longhand every day, at the machine.

We already have the soft jaws cut in steps for 6", 5.25" and 4.75" parts already in the machine and ready to go, 10 parts per load. We we running a batch of 5.25" drops earlier today at 12,000 RPM, 300IPM at 20% stepover. Most of the parts are only 1/4 to 1/2" over but have seen them as long as 1" oversized depending on what size pieces are cut from the bar so those parameters work safely up to 1" DOC.

The op didn't mention what material he is working with and I understand this isn't the catch all-solve all solution but thought I would throw it out as someone may benefit from it.

litlerob1 · May 15, 2017

Dave? Dave? are you saying that is quicker to remove metal from a round in a Mill than it is in a Lathe? Isn't that what the youngsters are for? Load, Unload, Load, Unload?

Just out of curiosity, why use a .5" Endmill instead of something bigger that can take more material?

R

gorrilla · May 15, 2017

Captdave said:
We already have the soft jaws cut in steps for 6", 5.25" and 4.75" parts already in the machine and ready to go, 10 parts per load. We we running a batch of 5.25" drops earlier today at 12,000 RPM, 300IPM at 20% stepover. Most of the parts are only 1/4 to 1/2" over but have seen them as long as 1" oversized depending on what size pieces are cut from the bar so those parameters work safely up to 1" DOC.

The op didn't mention what material he is working with and I understand this isn't the catch all-solve all solution but thought I would throw it out as someone may benefit from it.

View attachment 198702
View attachment 198703

No problem. HSM is not something I get to use much, so the results can be foreign to me at times.
This is the beauty of this forum. We have a multitude of people who MAKE A LIVING at this, and quite a few that have for some time. We get a LOT of experienced comments on just about anything anybody wants to know. Virtually none of it is wrong, but you do have to consider what the fellow posting was trying to convey, as well as what the responder was trying to get across. I appreciate your input. Hope it helped someone, and the OP may HAVE been cutting aluminum, he didn't say.
Glad to see I was not completely out of my mind about the jaws being cut to fit the part a bit. It amazes me sometimes what some folks will try to do if you don't specifically tell them one way or the other. Trying what your talking about in soft jaws, cut to fit, would work vastly better than trying to just throw a round piece in a set of hard jaws. YOU already know that, obviously. Otherwise, you wouldn't have went to the trouble. A newbie? He'll figure it out. Might take an end mill with it, but good decisions come from experience. Experience comes from bad decisions, often.

Booze Daily · May 15, 2017

Just add an extra facing pass in the lathe program.
It would be a helluva lot quicker.

Captdave · May 15, 2017

litlerob1 said:
Dave? Dave? are you saying that is quicker to remove metal from a round in a Mill than it is in a Lathe? Isn't that what the youngsters are for? Load, Unload, Load, Unload?

Just out of curiosity, why use a .5" Endmill instead of something bigger that can take more material?

R

I'm not in anyway saying its always the case but I can assure you its the safest way. We use to do them in the lathe years ago until someone....
1. forgot to reset the facing allowance in the program and threw out a part, damaging the door so bad that the door had to be removed and reworked and the glass replaced., $700 bucks for window and 1.5 days to repair and reinstall.
2. Cutting them on a manual band saw but getting them square and on size was a real time eater or see #1 above.
3. Selling the slugs on fleeBay totally sucked.
4. 1/2" endmills are cheap if you do break one, always have several in the machine but can't remember the last time one got broke.

They are generally sorting the next 10 while waiting for the 10 in the machine to finish. Normally we wait till we have 300-400 pieces to run at a given time.

EnderDRM · May 15, 2017

gorrilla said:
No problem. HSM is not something I get to use much, so the results can be foreign to me at times.
This is the beauty of this forum. We have a multitude of people who MAKE A LIVING at this, and quite a few that have for some time. We get a LOT of experienced comments on just about anything anybody wants to know. Virtually none of it is wrong, but you do have to consider what the fellow posting was trying to convey, as well as what the responder was trying to get across. I appreciate your input. Hope it helped someone, and the OP may HAVE been cutting aluminum, he didn't say.
Glad to see I was not completely out of my mind about the jaws being cut to fit the part a bit. It amazes me sometimes what some folks will try to do if you don't specifically tell them one way or the other. Trying what your talking about in soft jaws, cut to fit, would work vastly better than trying to just throw a round piece in a set of hard jaws. YOU already know that, obviously. Otherwise, you wouldn't have went to the trouble. A newbie? He'll figure it out. Might take an end mill with it, but good decisions come from experience. Experience comes from bad decisions, often.

I call it the "learn while you burn" program.

plastikdreams · May 15, 2017

What is the thickness of the current parts and what do you need it to be? What is the od? What is it made from?

This is really elementary stuff. How does what the bandsaw cut have anything to do with the finished part...unless it cut too small. :scratchchin:

zipfactor · May 17, 2017

plastikdreams said:
What is the thickness of the current parts and what do you need it to be? What is the od? What is it made from?

This is really elementary stuff. How does what the bandsaw cut have anything to do with the finished part...unless it cut too small.

Current thickness is ~7.2mm, final thickness 6.4mm. Material is 6061 aluminum.

The bandsaw cut thickness has to do with the problem as the CNC program is written to take off so much on each side. Unless I'm missing something, I need to run either an additional program on the mill or throw the parts on the lathe.

Elementary it is, I agree. I don't think anybody was debating that fact. I guess now I know next time to use another reference point instead of the top of the stock, that way I end up with the same thickness parts.

Facing Round Parts in CNC Mill - Rework

Cast Iron

Diamond

Cast Iron

Diamond

Cast Iron

Cast Iron

Cast Iron

Plastic

Stainless

Diamond

Titanium

Stainless

Titanium

Diamond

Stainless

Titanium

Titanium

Aluminum

Diamond

Cast Iron

Similar threads