Knurl on curved surface

[wojtek90]

hi 

I have a part which need to have knurl on top curves surface.

  90 degree groove  0.03 deep 0.125"  apart. See part and picture of groove.

How it should be programmed in Mastercam  what toolpath would be the best for it ? I have 90 degree Spot #9 chamfer cutter.

3-480-092-016.x_t

[AMCNitro]

I would do it with a slitting saw...

[#Rekd™]

Create the center lines for the knurl above the part in 2D mode in the pattern that is required. Then project them to the surface. Then use a contour toolpath with the Compensation type set to "Off" to follow the lines. Set you depth as required.

 

[wojtek90]

58 minutes ago, #Rekd™ said:

Create the center lines for the knurl above the part in 2D mode in the pattern that is required. Then project them to the surface. Then use a contour toolpath with the Compensation type set to "Off" to follow the lines. Set you depth as required.

 

Thank you for quick responce.

I like the idea but is depth will be constant on the curved surface even with 2D contour path?

[crazy^millman]

20 minutes ago, wojtek90 said:

Thank you for quick responce.

I like the idea but is depth will be constant on the curved surface even with 2D contour path?

The idea is to create the geometry projected to that surface and then drive from that curved geometry that is following the surface. You will want to switch to 3D and do like he said and you should be good to go. You will not normally see 3D as an option when you have 2D geometry, but when you have 3D geometry then 3D shows up as an option in the contour toolpath.

[Rstewart]

If this requires a sharp point that the bottom of the "V" a chamfer/spot/mill ain't gonna get it.  You could lay the part at a 45 deg angle and use a regular endmill.

 

I' done this before by using my machining center as a Shaper, that is as long as you have spindle orientation.  I ground a piece of HSS to a sharp point and it worked great in Aluminum (using AL tap magic).

[crazy^millman]

I was able to do what we said and toolpath in less than 5 minutes. Here is a screen shot of the Verify.

[#Rekd™]

Like Ron stated once you select the "projected" line the toolpath will recognize it as a 3D contour.

Use Lead In/Out to extend the start and exit of the projected lines.

You will notice that the depth options (Absolute/ Incremental) are grayed out as it is a 3D curve.

 

[crazy^millman]

6 minutes ago, #Rekd™ said:

Like Ron stated once you select the "projected" line the toolpath will recognize it as a 3D contour.

Use Lead In/Out to extend the start and exit of the projected lines.

You will notice that the depth options (Absolute/ Incremental) are grayed out as it is a 3D curve.

 

Only thing to add is the -.03 has to be either on the stock to leave on floors or in the depth on the linking page to get the .03 called out on the print since it is projected to the top surface of the part.  I also suggest using Model prep to fill the holes before projecting the lines on the top of the solid.

[#Rekd™]

I didn’t set the depth on that linking parameter photo! I had deleted the file so I was putting something together quickly!! In my original file I had the depth set to -0.03”.

Filling in the holes is a great suggestion that I hadn’t even thought of!

[crazy^millman]

6 minutes ago, #Rekd™ said:

I didn’t set the depth on that linking parameter photo! I had deleted the file so I was putting something together quickly!! In my original file I had the depth set to -0.03”.

Filling in the holes is a great suggestion that I hadn’t even thought of!

All good John just being the crazy person in the room is all.

[wojtek90]

7 minutes ago, 5th Axis CGI said:

All good John just being the crazy person in the room is all.

You guys are amazing. Thank you.

It would be to much if I will ask for Mastercam file with all what you showing.

[crazy^millman]

1 minute ago, wojtek90 said:

You guys are amazing. Thank you.

It would be to much if I will ask for Mastercam file with all what you showing.

No problem here you go. All I ask is you pass it on to others like i have done for many years on this forum.

Pass it on

Have a good night.

[wojtek90]

35 minutes ago, Rstewart said:

If this requires a sharp point that the bottom of the "V" a chamfer/spot/mill ain't gonna get it.  You could lay the part at a 45 deg angle and use a regular endmill.

 

I' done this before by using my machining center as a Shaper, that is as long as you have spindle orientation.  I ground a piece of HSS to a sharp point and it worked great in Aluminum (using AL tap magic).

 0.03 radius on the tip of the tool is OK. Thank you for suggestion.

 

 

[wojtek90]

7 minutes ago, 5th Axis CGI said:

No problem here you go. All I ask is you pass it on to others like i have done for many years on this forum.

Pass it on

Have a good night.

Thank you I got it.  Good night .Stay safe.