can i surface the underside of something with a woodruff cutter?

[cherokeechief79]

its just a straight angle.im having a hard time getting any toolpath to drive correctly using the top edge of the cutter or even to drive on the underside of a surface at all.

[JMahon]

If possible just use a 2d contour. And use linking parameters to get it to use the undercut side.

 

Or load up a file. I'll take a look

[Guest]

Of you're talking something like the underside face of a counter bore, chain the diameter, then drop your Z the thickness of the cutter

[gcode]

I beleive flowline and contour are the only 2 surfacing toolpaths than can machine an undercut

In both cases, you have to turn off gouge checking on the Gaps page to get it to work

[cherokeechief79]

Of you're talking something like the underside face of a counter bore, chain the diameter, then drop your Z the thickness of the cutter

thanks guys . I used wireframe ruled. and dropped the geometry the width of the cutter. I thought there might be a way of driving the upper edge of the tool with one of the new fancy surfacing paths. wireframe is one of the oldest and most dependable toolpaths of all .great toolpath with 0 retacts!

[Jayson Kramer]

Show us the surface you are trying to cut as there may be just a surface path to do it. I have my self done a lot of undercutting using woodroof cutters.

[Jim at Gentex]

Show us the surface you are trying to cut as there may be just a surface path to do it. I have my self done a lot of undercutting using woodroof cutters.

 

I also have an application where I abrade a variable width strip around the bottom surface of a polycarbonate lens using a dovetail cutter. 

I used a curve 5-axis toolpath with the edge of the abrade surface as the drive curve, the abrade surface itself as the tool axis control, and the side tilt value set to the angle of the dovetail cutter.

 

Works like a champ! 

 

As with any multiaxis application in Mastercam, there are usually several different ways to get there.

[cherokeechief79]

Show us the surface you are trying to cut as there may be just a surface path to do it. I have my self done a lot of undercutting using woodroof cutters.

sorry I cant post the part .ill try to draw up something similar.

[crazy^millman]

I beleive flowline and contour are the only 2 surfacing toolpaths than can machine an undercut

In both cases, you have to turn off gouge checking on the Gaps page to get it to work

 

Morph between 2 curves in 3 axis will handle it as well.

[crazy^millman]

its just a straight angle.im having a hard time getting any toolpath to drive correctly using the top edge of the cutter or even to drive on the underside of a surface at all.

 

 

I have dynamic contour these for about the last year and it does awesome. Had a bowl area on a part where it was taking 4 tools to machine it. The customer demanded off the shelf tooling to machine the shape. Each bowl shape on one part was taking 45 minutes to machine and the finish was about a 63. There were 3 bowls to cut and due to not being able to get the tools like I wanted and having to settle for small shanks the roughing tool was only holding up for about 2 parts. I designed a custom 3 flute full shape tool. I then dynamic contoured it and the run time was right at 5 minutes per bowl and the finish was about a 20. Everyone who looks at the parts asks me what lathe did I turn the bowls in and how did I fixture them for the lathe. Custom tool cost $400 a bowl. The saving per year on 10 parts per month was right at $50k. Guess what the custom quit demanding?

[Teh Bear without Brains kinda idiot]

I beleive flowline and contour are the only 2 surfacing toolpaths than can machine an undercut

~~~~~~~~~~~~~~

That`s far from true.

I make undercuts every day in 50 % of my parts making extrusion molds .

In extrusion it is a common feature

I make them using surface pocket and contour .

Once after you tried and got understanding what to do it is safe .fast and easy

Show me your part and  I will make an example toolpathes

[jlw™]

I have dynamic contour these for about the last year and it does awesome. Had a bowl area on a part where it was taking 4 tools to machine it. The customer demanded off the shelf tooling to machine the shape. Each bowl shape on one part was taking 45 minutes to machine and the finish was about a 63. There were 3 bowls to cut and due to not being able to get the tools like I wanted and having to settle for small shanks the roughing tool was only holding up for about 2 parts. I designed a custom 3 flute full shape tool. I then dynamic contoured it and the run time was right at 5 minutes per bowl and the finish was about a 20. Everyone who looks at the parts asks me what lathe did I turn the bowls in and how did I fixture them for the lathe. Custom tool cost $400 a bowl. The saving per year on 10 parts per month was right at $50k. Guess what the custom quit demanding?

I love stories like this. Being willing to pony up for good tools always pays in dividends. Trying to fight something with the wrong tools, in my experience, always ends in wasting money the cheap way and still buying the right tooling.

[cherokeechief79]

hard to believe that it took a week to get this from my standalone mc computer to here!

[cherokeechief79]

3865AS210-7 sample.mcx-8

 

disregard all but op 15. you can see I moved the geometry to the right and drove the tool from that position as I couldn't get the tool to drive on the correct side of the model

[Teh Bear without Brains kinda idiot]

cherokeechief79

 

Sorry I have only X7

So if you want my help please put in MCx-7 file

 

BR

[CJep]

I switched your tpath to a 3D wireframe,

Also sent the tool profile geom to a level,

This allows you to shift the tool so Y zero is at the top of the slot mill,

The green tpath geom is the across and the red is the along,