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:

NPT Threadmilling - Troubleshooting


colton_m
 Share

Recommended Posts

Hello,

Today I decided to try and define some NPT threadmills using the "threadmill" option in Mastercam 2018.

Previously I have defined my NPT threadmills as a "taper mill". This allowed me to define the tool in the exact shape as real life. I have been doing it this way for about two years with great success, everything makes sense and the code is good.

When I tried to define the same tool as an actual "threadmill" in Mastercam things started getting funny. I was able to define the tool to match exactly so everything looked good, When I toggle the toolpath display on I would expect both the old and new toolpaths to be identical. In reality when I use the tool defined as an actual "threadmill" the toolpath cuts undersize, by a lot.

If anyone could have a look and provide some suggestions that would be great.

- Colton

NPT THREADMILL TEST.ZIP

Link to comment
Share on other sites

Colton,

 

I took a quick look at this. It seems to me that it's the way MC is interpreting the diameter of the tool vs the angle. I got rid of the taper angle in the path and it works fine.  With an endmill it's using actual diameter (of shank) which is .375" (hence the .007" overcut you're using in the first path, because the cutting edge doesn't extend all the way to the shank) Where with the thread mill it's better taking into account the taper of the tool, using the tip size instead of shank size.

 

I hope this helps.

 

Caleb

Link to comment
Share on other sites
On 7/18/2019 at 3:41 PM, Manofwar said:

Colton,

 

I took a quick look at this. It seems to me that it's the way MC is interpreting the diameter of the tool vs the angle. I got rid of the taper angle in the path and it works fine.  With an endmill it's using actual diameter (of shank) which is .375" (hence the .007" overcut you're using in the first path, because the cutting edge doesn't extend all the way to the shank) Where with the thread mill it's better taking into account the taper of the tool, using the tip size instead of shank size.

 

I hope this helps.

 

Caleb

Its using the tip diameter on both. The reason the paths are different is because the tip diameter on the tools are different. If you make them the same, the paths come out identical.

 

To answer the question though.... your tools are different diameters in each operation, giving you a different tool path. 

Link to comment
Share on other sites
  • 1 year later...
11 minutes ago, Threept82 said:

Hi Guys,

Question,

I haven't thread milled an NPT hole in a very long time and feel silly but forgot how to find the size to program to.

1/2-13 program to .500

3/4-10 program to .750

1/8-27 NPT program to ?

Please advise.

Thanks

 

 

 

 

This what you are looking for?

 

image.png.a61a9fe1a6e67a2d5f76eba769ba2060.png

Link to comment
Share on other sites
  • 6 months later...

ok, I have never done threadmilling at all so I have some very basic questions:

When drawing my threadmill do I use the tip diameter or the top diameter?

When selecting the wireframe do I want the tap drill size or the final 1/2-14NPT size?

Is there a way to add cutter comp in the threadmill operation to make sure the threads finish correctly?

Link to comment
Share on other sites
1 hour ago, sharles said:

ok, I have never done threadmilling at all so I have some very basic questions:

When drawing my threadmill do I use the tip diameter or the top diameter?

Use the known diameter of the cutting edge. Top diameter (meaning tool shank if I understand yuour reference correctly) means nothing other than representation of what you're hanging onto.

1 hour ago, sharles said:

When selecting the wireframe do I want the tap drill size or the final 1/2-14NPT size?

Two options; 1) if you only have the minor diameter modeled, then you will need to override the size properties or 2_ if you have the major diameter modeled, pick that, then the size properties will be correct.

1 hour ago, sharles said:

Is there a way to add cutter comp in the threadmill operation to make sure the threads finish correctly?

Yes, just like a contour operation, select the type of comp you want. Computer = no G41/G42, Wear = G41/G42 and you will make relatively small adjustments in comp table at the machine, Control = G41/G42 and you'll need to put the Diameter/Radius (Depending on how your machine is set) in comp at the machine.

image.thumb.png.d5687b492baadd0a69b269c587500f28.png

HTH

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

Use the major diameter as drive geometry  ... see the thread definition in the Carmex Thread Wizard

Newer releases on MC have a dedicated thread mill

If you are using an old version, just define it as an endmill 

The thread mill toolpath has a wear option to output cdc

If you use the tip dimater to define your tool the toolpath will require minimal CDC to gate properly

If you use the major diameter you will cut an undersized thread and you can sneak up on finish size with CDC

 

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

Use the major diameter as drive geometry  ... see the thread definition in the Carmex Thread Wizard

Newer releases on MC have a dedicated thread mill

If you are using an old version, just define it as an endmill 

The thread mill toolpath has a wear option to output cdc

If you use the tip dimater to define your tool the toolpath will require minimal CDC to gate properly

If you use the major diameter you will cut an undersized thread and you can sneak up on finish size with CDC

 

Thanks, Gcode I am in 2022 so I am drawing my tool with the actual threadmill category and I selected "American National Pipe Thread", but for outside diameter you think I should use the top of our tapered threadmill instead of the bottom so that we can sneak up on it with cutter comp?

I did find the 'wear' selection' within the threadmill operation. Hopefully, it will pickup cutter comp correctly for our machines because I always have to select a lead in point whenever I use the simple 'contour' operation with cutter comp, but this toolpath does seem to start in the direct center of the hole before it arcs out and cuts the threads.

Should I have to mess with the 'thread pitch' inside the threadmill operation if I told it 14 threads per inch in the tool geometry?

And for "Number of active teeth" we are using a solid carbide tool not and inserted one, so there are 13 teeth...and so I put that in.

Thanks for everyone's help!

  • Like 2
Link to comment
Share on other sites
16 minutes ago, crazy^millman said:

Now I feel Old

you are old :whistle:

 

 

 

18 minutes ago, sharles said:

but for outside diameter you think I should use the top of our tapered threadmill instead of the bottom so that we can sneak up on it with cutter comp?

setting it to the top diameter is safer but will take longer to dial in

depending on thread size it could take as much as .030 CDC and you know

your operator will sneak up on it .002 or .003 at a time

 

 

I HATE this thread merge feature 

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

 

setting it to the top diameter is safer but will take longer to dial in

depending on thread size it could take as much as .030 CDC and you know

your operator will sneak up on it .002 or .003 at a time

 

then maybe it would be smart to set it say, .01 larger than the bottom diameter(.441) but not all the way at the upper .495 diameter...so they don't have so far to go????

Link to comment
Share on other sites

 

From my time at a die cast vent block company:

THREAD FORM THREAD DIA TOOL DIA LOC RPM SOFT RPM MED RPM HARD FEED SOFT FEED MED FEED HARD PILOT ROUGH STEP FINISH STEP ENTRY ARC CUT DEPTH
        200 SFM 150 SFM 120 SFM         30% 20%    
0-80 0.0600 0.044 0.250 17362 13022 10417 3.1 2.30 1.9 0.047 0.0020 0.0013 0.0033 -0.5000
2-56 0.0860 0.064 0.156 11937 8952 7162 3.1 2.30 1.9 0.07 0.0024 0.0016 0.0040 -0.5000
4-40 0.1120 0.080 0.500 9549 7162 5730 3.1 2.30 1.9 0.089 0.0035 0.0023 0.0058 -0.5000
5-40 0.1250 0.093 0.500 8214 6161 4929 3.1 2.30 1.9 0.1094 0.0023 0.0016 0.0039 -0.5000
6-32 0.1380 0.098 0.625 7795 5847 4677 3.1 2.30 1.9 0.116 0.0033 0.0022 0.0055 -0.5000
8-32 0.1640 0.115 0.250 6643 4982 3986 3.1 2.30 1.9 0.1417 0.0033 0.0022 0.0056 -0.5000
10-24 0.1900 0.130 0.250 5876 4407 3526 3.1 2.30 1.9 0.161 0.0044 0.0029 0.0073 -0.5000
10-32 0.1900 0.130 0.250 5876 4407 3526 3.1 2.30 1.9 0.1693 0.0031 0.0021 0.0052 -0.5000
1/4-20 0.2500 0.180 0.480 4244 3183 2546 3.1 2.30 1.9 0.2188 0.0047 0.0031 0.0078 -0.4500
1/4-28 0.2500 0.180 0.480 4244 3183 2546 3.1 2.30 1.9 0.2205 0.0044 0.0030 0.0074 -0.4500
5/16-18 0.3125 0.235 0.625 3251 2438 1950 3.1 2.30 1.9 0.277 0.0053 0.0036 0.0089 -0.6250
3/8-16 0.3750 0.290 0.789 2634 1976 1581 3.1 2.30 1.9 0.332 0.0065 0.0043 0.0108 -0.7500
7/16-14 0.4375 0.300 0.860 2546 1910 1528 3.1 2.30 1.9 0.368 0.0104 0.0070 0.0174 -0.8250
1/2-13 0.5000 0.350 0.846 2183 1637 1310 3.1 2.30 1.9 0.4375 0.0094 0.0063 0.0156 -0.8250
5/8-18 0.6250 0.240 0.750 3183 2387 1910 3.1 2.30 1.9 0.5938 0.0047 0.0031 0.0078 -
1.0-8 1.0000 0.488 - 1565 1174 939 3.1 2.30 1.9 0.9219 0.0117 0.0078 0.0195 -
1.125-18 1.1250 0.250 0.638 3056 2292 1833 3.1 2.30 1.9 1.065 0.0090 0.0060 0.0150 -
M4X.7 0.1575 0.115 0.250 6643 4982 3986 3.1 2.30 1.9 0.1285 0.0044 0.0029 0.0073 -0.2400
M5X.8 0.1969 0.120 0.312 6366 4775 3820 3.1 2.30 1.9 0.166 0.0046 0.0031 0.0077 -0.3000
M6X1.0 0.2362 0.170 0.500 4494 3370 2696 3.1 2.30 1.9 0.1969 0.0059 0.0039 0.0098 -0.4750
M8X1.25 0.3150 0.235 0.625 3251 2438 1950 3.1 2.30 1.9 0.266 0.0073 0.0049 0.0122 -0.6000
M12X1.75 0.4724 0.360 0.875 2122 1592 1273 3.1 2.30 1.9 0.40625 0.0099 0.0066 0.0165 -0.8500
M20X1.5 0.7874 0.488 1.500 861     2.03     0.7343 0.0080 0.0053 0.0133 -1.4500
M20X2.5 0.7874 0.488 1.500 861     2.03     0.7343 0.0080 0.0053 0.0133 -1.4500
M24X3.0 0.9449 0.488 1.500 861     2.03     0.8268 0.0177 0.0118 0.0295 -1.4500
                             
                             
1/16-27 NPT 0.3125 0.222 0.461 3441 2581 2065 3.1 2.30 1.9 0.25 0.0094 0.0063 0.0156 -0.4500
1/8-27 NPT 0.4050 0.284 0.510 2690 2017 1614 3.1 2.30 1.9 0.34375 0.0092 0.0061 0.0153 -0.5000
1/4-18 NPT 0.5400 0.335 0.691 2280 1710 1368 3.1 2.30 1.9 0.4375 0.0154 0.0103 0.0256 -0.6750
3/8-18 NPT 0.6750 0.335 0.691 2280 1710 1368 3.1 2.30 1.9 0.5625 0.0169 0.0113 0.0281 -0.6750
1/2-14 NPT 0.8400 0.450 0.820 1698 1273 1019 3.1 2.30 1.9 0.7187 0.0182 0.0121 0.0303 -0.8000
3/4-14 NPT 1.0500 0.450 0.820 1698 1273 1019 3.1 2.30 1.9 0.906 0.0216 0.0144 0.0360 -0.8000
1.0-11.5 NPT 1.3150 0.488 - 1565 1174 939 3.1 2.30 1.9 1.1563 0.0238 0.0159 0.0397 -
1.25-11.5 NPT 1.6600 0.488 - 1565 1174 939 3.1 2.30 1.9 1.4844 0.0263 0.0176 0.0439 -
1.5-11.5 NPT 1.9000 0.488 - 1565 1174 939 3.1 2.30 1.9 1.7188 0.0272 0.0181 0.0453 -
                             
                             
1/16-28 BSPT 0.3040 0.215 0.550 3553 2665 2132 3.1 2.30 1.9 0.25 0.0081 0.0054 0.0135 -0.5250
1/8-28 BSPT 0.3830 0.215 0.550 3553 2665 2132 3.1 2.30 1.9 0.3125 0.0106 0.0071 0.0176 -0.5250
1/4-19 BSPT 0.5180 0.335 0.700 2280 1710 1368 3.1 2.30 1.9 0.4375 0.0121 0.0081 0.0201 -0.6750
3/8-19 BSPT 0.6560 0.335 0.700 2280 1710 1368 3.1 2.30 1.9 0.5625 0.0140 0.0094 0.0234 -0.6750
1/2-14 BSPT 0.8250 0.450 0.821 1698 1273 1019 3.1 2.30 1.9 0.75 0.0113 0.0075 0.0188 -0.8000
5/8-14 BSPT 0.9020 0.450 0.821 1698 1273 1019 3.1 2.30 1.9 0.828 0.0111 0.0074 0.0185 -0.8000
3/4-14 BSPT 1.0410 0.450 0.821 1698 1273 1019 3.1 2.30 1.9 0.969 0.0108 0.0072 0.0180 -0.8000
  • Thanks 4
  • Like 3
Link to comment
Share on other sites

I deal with too many models that come from a variety of often terrible sources so I have used point to define all my threadmill toolpaths for longer than a decade.

I define my threadmills exactly how my source defines them so when the dudes on the floor get my tool list it says the same thing on the tin. My current source (JBO) defines the tip diameter and the shank diameter along with cut length. I just plug all that in to mastercam along with the taper (1.7833) into every npt I make (usually 1" to 2" npts) and I start with the OD tube diameter defined on the charts and work from there. Depending on the machine they typically end around -.002" to -.014" comp. The inserted npt threadmills we use occasionally just suck balls so we end up with a lot more comp than the solid carbide ones.

Link to comment
Share on other sites
32 minutes ago, gms1 said:

The inserted npt threadmills we use occasionally just suck balls so we end up with a lot more comp than the solid carbide ones.

Try Carmex Spiral Mills Spiral Mill-Thread | Carmex

We do hundreds of 1-11.5 NPT's a month and these work really well

On a rigid machine with good through coolant you can get 40 to 50 holes from a set of inserts with a 30 to 45 second cycle time

 

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

We recently did a job where these tools really impressed me

Ø3.750 x 8UN 2B x 5.750 deep 16 places in 321 stainless steel

We used a thru coolant shell mill that held 9 inserts

We put it on a thru coolant shell mill arbor

3 passes  -.015 , finish, then spring

The tool did all 16 holes with one set of inserts 

The first hole required -.002 CDC, the last hole -.004

I was dreading this operation but it ran completely trouble free 

  • Like 2
Link to comment
Share on other sites
5 hours ago, gcode said:

Try Carmex Spiral Mills Spiral Mill-Thread | Carmex

We do hundreds of 1-11.5 NPT's a month and these work really well

On a rigid machine with good through coolant you can get 40 to 50 holes from a set of inserts with a 30 to 45 second cycle time

 

We use a combo of tungaloy, kennametal and vardex insert thread mills and I can't stand any of them. I am gonna give these a shot thanks man.

  • Like 1
Link to comment
Share on other sites

Use the Carmex Tool Wizard to calculate feeds and speeds

run it through and post the feeds and speeds. 

I do that so I know the correct feed rate comped to the ID of the tool path

 

43 minutes ago, gms1 said:

We use a combo of tungaloy, kennametal and vardex insert thread mills

The guys on the floor call these tools "slappers" cause that's how they sound in the cut 

Link to comment
Share on other sites

Just wanted to thank everyone for their help and input. We did a little testing in aluminum before running the real holes in steel and found out mastercam wanted the thread pitch diameter, and so I changed my tapdrill arcs to what mastercam wanted but a little smaller so the operators could sneak up on it and it worked really well.:cheers:

  • 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...