Arc Clockwise lead in - easy way?

[sweinberg]

Hi All,

 

New user, so hopefully this is in the right place.

 

I've seen in various places that it is advantageous to lead in with a clockwise arc when climb milling (essentially rotating the mill around a single point on the edge of your part [or probably NEAR it in real life]). That way you get a more uniform thick to thin chip profile, and reduce tool shock.

 

However, Mastercam only gives an option for a CCW lead in, as far as I can see (and negative values don't work). I've had some success adding a short line with a very short right angle to where I want to lead in (the mill comes in to the edge of the angle, then curves around the corner, essentially giving me what I want), but it doesn't work in all situations, and it's often easier to pick up the geometry with the solid options, rather than 2D, which I don't think this works with.

 

So:

 

A) Is there an easy, or 'proper' way to get a CW lead in?

Is there some advantage to a CCW lead in that I should be considering? (I generally use it when leading in from inside a pocket instead of a straight perpendicular lead in, but I can't say with certainty it matters - or when it just makes more sense based on the stock and room in my machine).

 

Thanks in advance.

[Del.]

Welcome to the Forum. You will most likely get more responses by putting this post in the industrail forum

[sweinberg]

Thanks for the tip.

 

I assume I can't move it, right? So I should just create a copy?

 

I just don't want to get into trouble with the mods on my first day, so I want to make sure...

[Del.]

Thanks for the tip.

 

I assume I can't move it, right? So I should just create a copy?

 

I just don't want to get into trouble with the mods on my first day, so I want to make sure...

 

 

One of the mods can just move it for you.

[MotorCityMinion]

I saw a video about this some time ago. Either Sandvick or Seco, not sure. Anywho.. the HSM toolpaths such as OPTI_XXX, adapative clearing, Volumill, all use this aproach when they can.

AS far as 2d, I have not seen an easy way to acomplish this. Modify the geometry (CHAIN), then use a staight on entry will work but that is way too much hassel for most jobs IMO.

[PeterM]

It's not super simple, but here is how I do it. Create the lead in/lead out arcs as you would like to see them cut. Then chain the geometry, which can be a pain. In the cut parameters page turn off infinite look ahead. This allows Mastercam to ignore the crossing geometry.

[sweinberg]

Didn't know about infinite look ahead. Thanks.

 

About the arc, I'm not really sure how I'd draw it, what with the offset, and the fact that I want the tool to rotate around a single point. However, what might even be simpler is what I mentioned in the first post, if you extend a small line out from your start point, then take a right turn (really small), then your tool will take a CW turn around the corner you've now created [assuming you round sharp corners, which I almost always do]

 

You could probably just create a corner at your actual lead in point, but I want to be careful about nicking the material.

 

I'm hoping there's a better way, and one that works with solid geometry (so I can grab a more complex outline of a face, for example, without going through each line in the chain, selecting them in order).

[NOTW Programmer]

Thats pretty neat, too bad you gotta mess with Geometry, would be nice if CNC Software would add it.

[sweinberg]

NOTW Programmer, In the case in your thumbnail, I'd probably make the first line (perpendicular to your cut) equal to the radius of the tool (barring other factors). That way, the corner is one radius from the edge, and that's the point the tool rotates around, giving you a nice full rotation into the part.

 

Originally, I was assuming the lead in was tangent to the cut (e.g., in your simple case, had you led in tangent to a corner).

[Thoob]

This has been discussed here for awhile. The fact its not implemented is pure laziness on CNC Softwares part. No if ands or buts. That video you mention is Sandvik. Its here.

I do just as the video says, create an arc and follow it.

[jeff]

Yeah I've seen that video before, makes total sense too.

[specv]

Offset the geometry by the diameter of the cutter and chain it using right and not left comp. that way your lead in will be the opposite side of the line.

[sweinberg]

Yeah, I've seen that video. But also other places. I know CNCcookbook covered it, and I think I've seen it 2 or 3 other places as well.

 

I've explained earlier that I'm not sure exactly how you'd rotate around a single point with an arc, assuming that you want to use an offset for your mill (i.e. your path is the final surface, not tool center). I find a corner works well, though.

[jeff]

Offset the geometry by the diameter of the cutter and chain it using right and not left comp. that way your lead in will be the opposite side of the line.

Yeah there are workarounds to make this work, but we shouldn't have to offset or create any new geometry for a lead in/out.

[specv]

I agree, the instead of offsetting geometry set stock to leave at the diameter of the cutter. Otherwise use the dynamic toolpaths.

[Bill Craven]

Greetings all,

 

I work for Sandvik and several times a year we offer classes on how to leverage Mastercam to produce these types of toolpaths.

I will attempt to attach an example file and PowerPoint slide from my presentation.

This same technique also works for Lathe

BTW: I have had conversations with a couple of the developers at Mastercam and it is on their list, I just don't know when it will be implemented.

Roll into cut Mastercam.zip

[Chris Rizzo]

That's great Bill, thank you for sharing that!

 

Where are you based? Sandvik has done some presentations at our college, recently the hole-making one. They provide a lot of nice test tooling for us too.

 

p.s. I like your computer specs, but I have ya beat with 100x less ram (no mastercam however, just hand written games)

[Bill Craven]

Thanks Chris.

 

I am currently located in New Jersey but I am in the process of moving to Gcode's neck of the desert in southern California: Rancho Cucamonga, Fontana.

 

I was up in your neck of the woods earlier in the year to do a class at a customer's and stopped by your school, but you were off that day. We drove on up to Seattle and did a one day seminar at Renton Technical College for educators teaching Mastercam organized by Fransisco. It was a good trip, sorry I missed you.

[sweinberg]

Hi Bill,

 

I'm wondering if there's an advantage to using a curve, as shown in your picture, rather than a sharp corner (at the part edge if you want to be exact, but I'd put it very slightly out to be sure you don't ding the finish of the adjacent wall). This is assuming that you round sharp corners.

 

It's probably not a big difference either way, but this seems technically more correct to me, and also I find it slightly simpler to do.

[Bill Craven]

An interesting idea Mr. Sweinberg (or probably Mr. Weinberg). You seem to have a good grasp of the thick to thin chip profile to reduce shock to the tool concept. This is Sandvik's mantra for increased tool life, especially in Heat Resistant Super Alloys with carbide.

 

I hadn't ever tried a straight line move before, but I have now and it appears to work just as well and is more technically correct. I also think that in many cases it would be easier to add the line segment. (or line segments by locking the length and angle field when creating the segments).

 

Kudos and my thanks to you.

 

 

This is why I love the forum so much. I come here everyday to learn.

[sweinberg]

You're welcome. And, yeah, it's S. Weinberg.

 

I'm actually new to the game. I've been designing stuff for a couple of years, but I'd never really touched CAM (or a CNC machine) until February of this year. Obviously still learning every day (I expect I probably will never stop learning). Thought of the corner thing, but never really got it to work all the time until Peter M gave the tip off to turn off infinite look ahead.

 

Great tip videos by the way by Sandvik. Very much enjoyed them, and looking forward to any more that come out.

 

One thing I'm not sure about is if I can do this type of trick when using solid geometry instead of sketch geometry (I do turn on edge curves when loading my solids, but the selection process is different - it's usually much easier to select a somewhat complex chain with solid geometry). [Note, I only have a level 1 licence, so none of the more advanced 'solid' toolpaths - I'm only talking about selecting the geometry).

When I create the additional lines, I don't know of any way to combine that with the solid geometry as one tool path. Any tips?