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:

Suggestions for cutting gage pins


Recommended Posts

I have the task of cutting some gage pins to length for a special inspection fixture, about 8 different diameters, total quantity of 120 pins. We do not have a surface grinder. Current method consists of handheld Dotco grinder with a cut off wheel and then using VF2 to trim to length with a jig grinding pin. Cutting the pin to rough length with a handheld tool leaves something to be desired as cut off length is not consistent. I could put the Dotco grinder in the lathe by making a special bracket to hold the grinder, put the pin in a 5C collet and then turn on spindle and grinder and cut that way. But would a Cermet part off insert be a better way? I don't have any experience with using a Cermet insert.

And unfortunately, I do not have the option of starting from raw stock and cutting and grinding and then send out to heat treat.

 

Thanks, LeoC

Link to comment
Share on other sites

Yes, wire EDM would have been one of my first choices, but we don't have access to one of those. I don't even think they budgeted enough time for a wire EDM shop to cut them, turn around time that is.

This is one of those jobs where the people who quoted it didn't ask the people who actually have to do the task for any input.

LeoC

Link to comment
Share on other sites

Waterjet.  I can say that now that we have a Protomax and are finding all kinds of uses for it.  I recently had to cut about 200 1mm dia x 50mm long tubes without leaving a burr on the id.  Worked beautifully.

Link to comment
Share on other sites
13 hours ago, Matthew Hajicek - Singularity said:

I've made parts from gauge pins, when the OD was critical and the 52100 steel was appropriate.  Just mill it with carbide.

I'm with Matt. Carbide is roughly 70-80 HRc. Take light depths of cut, maybe 0.005-0.010 per pass, and just do a "zig-zag in depth, to move through the material. No need to grind with a grinding bit, unless you're requirement is for the ground finish on the cut-end of the gauge pin. Cutting with carbide should be much quicker, and you could likely "gang" these parts together, if you have a group of pins with the same length, using pockets in soft-jaws. (Cut in X or Y, drop down your depth-of-cut in Z, and reverse the cutting direction to go the opposite way, then repeat.)

If you hold the pins "on the side of the jaws" (as opposed to sticking "straight up"), you could slot-through the side of the pin. So, instead of machining away the entire material, you could just have to cut through the diameter, making slotting passes.

200-400 SFM, and 1-2% of the Tool Diameter, "per tooth".

  • Like 2
Link to comment
Share on other sites

Thanks for all of the great suggestions. I had talked to Iscar and Kennametal and am going to try a PCBN insert. I will post the results of how that goes, they are supposed to show up today. I had not thought of the high feed end mill, I will order some of those also in case the inserts do not work.

This user name is quite new, the shop I had worked before had closed the machine shop during the pandemic, so I had to find a new job after 15 years there. We use Fusion 360 and Mastercam here for our 5 axis gantry mill. I have always considered the eMastercam forums as a valuable source of intelligent information and again, thanks for the suggestions.

 

LeoC

Link to comment
Share on other sites

Update:

               Used an Iscar PCBN 3mm wide cut off insert using 325 SFM with a feed of .0008 using CSS. Broke the insert on first part, although it cut the pin very cleanly. I am wondering if it broke because of the tool not being centered correctly. I have attached pics of insert and pin. If I measure the nub diameter, it is about .020". Contacted Iscar rep for further suggestions. Helical feed mills should arrive on Tuesday.

 

LeoC

 

 

broken insert.jpg

pin with nub.jpg

Link to comment
Share on other sites
19 hours ago, socalsurf said:

Update:

               Used an Iscar PCBN 3mm wide cut off insert using 325 SFM with a feed of .0008 using CSS. Broke the insert on first part, although it cut the pin very cleanly. I am wondering if it broke because of the tool not being centered correctly. I have attached pics of insert and pin. If I measure the nub diameter, it is about .020". Contacted Iscar rep for further suggestions. Helical feed mills should arrive on Tuesday.

 

LeoC

 

 

broken insert.jpg

pin with nub.jpg

You might consider:

  • Yes, Center-height of the tool, could play a role. Should be as close to perfect as possible.
  • Try using RPM, instead of CSS. The "ramping" can have a big effect as you get close to "zero", and will be limited by your G50/Max. RPM line anyway.
  • Might consider starting at 0.0008 IPR, but only going down to about 0.080" Diameter, and then dropping down to 0.0002-0.0004" per revolution
  • If you continue to chip the inserts, consider dropping SFM by 50-75. (Try 250, or 275 SFM)
Link to comment
Share on other sites

Update 2:

                  Contacted Iscar after first insert broke, they suggested raising tool .007" and lowering the feed halfway through the cut to half the previous feed rate, so from F.0008 to F.0004, also ramped up max spindle speed to 4K. Worked great, no visible nub, very clean cut, and then on the 5th part, it chipped, this time on opposite side.  Since I only had two inserts on hand due to the cost, had to look for another option. I liked the lathe method because it was fast, 20 second cycle time and easy to load. So after seeing comments about just trying carbide, I used what I had, standard Haas 3mm cut off insert, HCI-3R, 3mm Carbide Cut-Off Insert, Grade HU30 - Pack of 10 (haascnc.com) . Ran it at 200 SFM and F.0008, used coolant and CSS, worked very well, not as clean as a cut but reliable. Since I have so many parts to cut in a short time, a reliable process was vital. I will just need a slight touch up on the bench grinder and they will be good to go. 

                Thanks again for all of the suggestions.

                                                                                  LeoC

 

 

Link to comment
Share on other sites
On 5/15/2022 at 3:41 PM, socalsurf said:

I have the task of cutting some gage pins to length for a special inspection fixture, about 8 different diameters, total quantity of 120 pins.

I would farm them out to a tool grinder.

They have tools built for this kind of work

Link to comment
Share on other sites
On 5/23/2022 at 4:04 PM, socalsurf said:

. I am wondering if it broke because of the tool not being centered correctly.

It broke because the RPM of the spindle is near zero at Ø.020

The insert cannot cut at those speeds

I'd stop a little before that and break it by hand.

  • Like 1
Link to comment
Share on other sites
2 minutes ago, gcode said:

It broke because the RPM of the spindle is near zero at Ø.020

The insert cannot cut at those speeds

I'd stop a little before that and break it by hand.

The other possible solution would be to not use CSS, use RPM mode only, and then reduce the feed, starting at about 0.080" Diameter, down to about 0.0004 IPR, and then at 0.040" diameter, reducing to 0.0002 IPR. Also, possibly increase the SFM by 25-50, and see if that helps at all. What color were the chips coming off at your current programmed SFM?

But I also like G-Code's advice to stop early, leaving the part connected, and breaking it off by hand. Either way, you will need to do some clean-up/finishing, unless that part of the pin is hidden in the fixture, and you can live with it.

I'd also suggest reprogramming the part-off code, to "plunge in" about 0.060", pull-back for clearance, and then add a "chamfer" move, from out-to-in, to help push any burr formed towards the pin center. If you put a 0.01-0.02" chamfer, that would be plenty. Might want to program at 35-degrees, or 40-degrees, instead of 45-degrees, to help with pushing the pin into the hole, if the installation will be permanent.

After cutting the chamfer, then proceed with the part-off cut, in stages, where you reduce the Feed-per-Revolution accordingly, or stop early, and hand-break the part.

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...