Milling glitch?

[Thad]

MC doesn't account for the corner radius on the tool. I have proven this by milling a pocket that is shallower than the size of the corner radius. In this instance, MC *should* compensate for the diameter of the cutter at that particular depth. On a 1.0 cutter with .25 corner radius going .08 deep, MC should *really* be compensating for a .867 dia cutter.

 

I have uploaded a file (corner rad.mc9) to the MC9 files directory on cadcam's FTP that demonstrates this. In this file, I have a pocket in which one of it's walls shares the edge of the part. When verified in the top view, if MC compensated for the corner radius, there would be no "radiused lip" (on the wall at X0) remaining after milling. If MC doesn't take into consideration the corner radius of the tool, that is not a good thing.

 

Thad

[McRae]

Thad,

 

Funny you should think this as I extensivly use Bull mills (Sandvik Coromill 300 program) and I find that Mastercam does account for all the radius values at various depth of cuts.

 

Let me see the file and then get back.

[McRae]

Thad,

 

Check Revised file (MFGENG) and then use verify. You will see that there is a radius to the outer contour and that the cutter is leaving the step that you want along the edge. I redefined the verify settings for the stock that you will see. Also look at the part in isometric, easier to visualize.

[ROB]

i looked at the file and it looks good to me,

it its compensating for the radius at the corner.

try dynamic and step mode, and zoom in at the corner and you will see.

[Thad]

Andrew,

 

I'm off for the weekend now so I'll have to check it out on Monday. But just for conversation sake, if the cutter leaves any step along the edge, then it is not compensating for the corner rad. I didn't want a step. This is not a real job either. It's just the easiest way that I could show that it doesn't compensate for the corner radius. If you programmed that same toolpath with a flat bottom tool, the bullnose that I used, or even a ball nose, you'd get the same X value, as it cuts along that wall, in all 3 posted programs. That means that it isn't taking the corner radius into consideration. As another example, if you really want to put it to the test, machine a pocket of some simple nominal dimensions that is shallower than your corner radius and then measure the pocket when you're done. It will not be the correct size. It will be smaller.

 

Do you do 3D work with bullnose cutters? Perhaps it only does this in a 2D arena.

Thad

[Thad]

Which file looks good, Rob? The original one I put up or the modified one by Andrew? Man, now I wish I wouldn't have left work early!

 

Thad

[McRae]

Then it is an open pocket!

 

We will resume Monday.

 

Andrew

[ROB]

yeah!

you guy's have a nice weekend!

[McRae]

Thad,

 

When "2"D pocketing the machine can only see the contour that you are moving around and then to apply an axial compensation for any tool radius. By saying that you want the "Edge" open, then I suggest to use "Open Pocket".

 

Also see in my file how I offset the contour to give teh .08 depth of cut, and used the corners of the intersecting lines as the stock definition.

 

I have not tried with a solid but I think it would give the same result.

[gstephens]

quote:

---

MC doesn't account for the corner radius on the tool. I have proven this by milling a pocket that is shallower than the size of the corner radius. In this instance, MC *should* compensate for the diameter of the cutter at that particular depth.

---

Why?? How does Mastercam know whether you want to cut with the eside of the tool or at some (infinite number)point along the corner radius? Are you looking for it to automatically offset based on an incremental depth from the geometry? I guess that would be nice; however, there has been a quite acceptable workaround for a LONG time... just chain the geometry at the tangecy at the bottom of the radius, and give it a NEGATIVE xy stock to leave equal to the corner radius. Works perfectly every time, and won't require an additional type of pocket and contour toolpath.

 

I can just see trying to explain Standard/Open/Facing/Island Facing/PARTIAL CORNER RADIUS options to a bunch of people who have never run CAD/CAM before.

 

JMNSHO

 

Oh BTW, I've put corner rad-g.mc9 on the FTP which runs this fine using surfaces (need level 3) with the appropriate settings.

 

[ 08-26-2002, 01:40 PM: Message edited by: gstephens ]

[Thad]

Andrew,

 

My intent is not to cut an open ended pocket. If you cut a pocket that was shallower than the corner radius of your tool, then you backplotted it and verified it, you would not even give it a second thought because everything "looked" OK. But when you cut it, you'd see that it did not cut the geometry correctly. Since you cannot measure in the verify mode, I came up with this example to *show* you how it wasn't compensating. The only way that I could think of to *show* you this is to cut a pocket where one wall of the pocket shares the edge of the part. They are exactly the same plane, therefore the bottom of the pocket should be perfectly flat and the end result would look like an open pocket. But it doesn't. Thus the "radiused lip" on the edge that shares the pocket wall and edge of the part.

 

Clearly, my way of describing this is not making sense you the readers. So, forget everything that I have said and try it. Cut a pocket in the middle of a part where the depth is less than the corner radius of your tool and then measure the pocket. The pocket will not be diminsionally correct. It will be smaller. The larger the corner radius, the smaller the pocket will be. Therefore, MC did not account for the corner radius of the tool. Period! The proof is in the pudding.

 

Unfortunately, I'm not at work today to look at your file.

 

Thad

[Thad]

gstephens,

 

quote:

---

Why?? How does Mastercam know whether you want to cut with the eside of the tool or at some (infinite number)point along the corner radius?

---

How does MC know how to cut *anything* that you tell it. It is a CAM system and based on the information it is given...tool dia, corner radius, depth of pocket..it figures it out.

 

quote:

---

Are you looking for it to automatically offset based on an incremental depth from the geometry?

---

If the pocket depth is shallower than the tool's corner radius, then yes. I expect the CAM system to cut the geometry dimensionally correct. If this is what it takes to accomplish that, that's what I expect.

 

quote:

---

I guess that would be nice;

---

It is nice! Gibbscam does it and who knows what other systems do it. (Not a slam on MC).

 

quote:

---

however, there has been a quite acceptable workaround for a LONG time...

---

Workaround? Only "problems" require workarounds.

 

quote:

---

just chain the geometry at the tangecy at the bottom of the radius, and give it a NEGATIVE xy stock to leave equal to the corner radius. Works perfectly every time, and won't require an additional type of pocket and contour toolpath.

---

Are you sure? Have you measured it? This will only work if you have a full 90 degree radius on the edges of the pocket, i.e. a .250 deep pocket with a .250 radius. AND, if that *is* the case, there is no need to use "special" geometry or cut with negative stock. Just cut it like you normally would.

 

With an .08 deep pocket and a .250 radius your method will not work. Some more math has to be done. This is my point. These "extra" calculations should be done by the CAM system. Either 1) How far will I have to offset the geometry so a .250 corner radius will cut an .08 deep pocket to the correct dimensions or 2) How much negative stock should I give it to cut an .08 deep pocket with a .250 corner radius to the correct dimensions?

 

quote:

---

I can just see trying to explain Standard/Open/Facing/Island Facing/PARTIAL CORNER RADIUS options to a bunch of people who have never run CAD/CAM before.

---

I hear ya! Drawing a line seemed to be a bit much for some of the guys who were in *my* MC class.

 

Thad

 

[ 08-27-2002, 09:39 AM: Message edited by: thad ]

[McRae]

Looking at it from a top plane perspective - here is what I found.

 

The axial cutcomp that you are looking for is not a countour option. I would offer the solution as a surface-pocket routine to give what you need. These are the toolpaths that I am using with the bull_mills and the axial compensation that you describe is clearly coming out in my part. However the latest FKIA (Fu--ing Know It All) post tone of your two previous posts has Pi$$ed me off and so I say Good Day!

[Guest CNC Apps Guy 1]

quote:

---

However the latest FKIA (Fu--ing Know It All) post tone of your two previous posts has Pi$$ed me off and so I say Good Day!

---

DOH!!!!!

[Roger Peterson]

The surface pocket toolpath is the answer. A 2D pocket is just that 2D. The situation can change many times over the length of a chain, by chaining a 2D contour mastercam doesn't know if the geometry is in an open area or next to a vertical wall you don't want to gouge into. Although the option would be convenient at times.

 

My two cents worth, darn it now I can't afford diapers!

 

[ 08-26-2002, 03:52 PM: Message edited by: Roger ]

[Thad]

quote:

---

However the latest FKIA (Fu--ing Know It All) post tone of your two previous posts has Pi$$ed me off and so I say Good Day!

---

Andrew,

 

You're reading too much into it. We seem to not be understanding each other so I'm just trying to get my point across.

 

Thad

[gstephens]

quote:

---

If the pocket depth is shallower than the tool's corner radius, then yes. I expect the CAM system to cut the geometry dimensionally correct. If this is what it takes to accomplish that, that's what I expect.

---

This is ASSUMING that the chained geometry is at the TOP of the pocket and that you are using the incremental depth to define the whole depth of the pocket. Not at all the way any of the other toolpaths work in Mastercam.

 

Here's a situation for you (and GibbSCAM if you still have access to that tripe) Pocket depth=.15, Tool nose radius = .25, Islands inside the pocket with height=.063, Multiple depth cuts .03 max cut. (pocket-g.mc9 on the FTP)

 

quote:

---

Workaround? Only "problems" require workarounds.

---

Not true in the least. I can't tell you how many times I just can't seem to get [any] CAM software to cut EXACTLY the way I want. So I have to model my toolpath and chain cutter center with no comp and voila, exactly what I want. All systems have inherent limitations. Workarounds are for those times when you run up against them.

 

quote:

---

Are you sure?

---

Quite.

 

quote:

---

Have you measured it?

---

Many times.

 

quote:

---

This will only work if you have a full 90 degree radius on the edges of the pocket

---

Incorrect. Notice I said the BOTTOM tangency (take a look at the pocket-g.mc9 file). No "extra calculations" required. I've been doing it this way for about 14 years now (since v2.something) and have never had a problem.

[Jack Mitchell]

Just a minor brief on cutter comp,

 

Application is to cut a 2” square pocket.

Machine zero is the center of this pocket.

 

G43 H01 X0 Y0 Z2.0 S1000 M03 M08

Z.1

G01 Z-.08 F.002

G01 G41 X0 Y-1.0 D01 F.025 (still with me?)

X1.0

Y1.0

X-1.0

X.25

G01 G40 X0 Y0

 

What I teach is that you program the actual contour of the part.

Cutter radius compensation will react correctly by establishing the basic part size control that cutter comp is meant to do. – it will give me (the operator, the ability to make a part in tolerance).

If the tool has a bullnose or a ballnose or a chamfer – this will occur naturally.

Which is to say (we do not deal with other things or problems) if the part is 2” square then everything is correct. – if the part is smaller than 2” square then we obviously did not go deep enough with our cutter.

 

Outside of this incredibly crude example – this workpiece needs to be surfaced.

Surfacing entertains a completely different set of circumstances; these are entirely predictable through trial & error. It’s how we learn.

 

If the crude example did not work accordingly – Then I guess I really don’t know so much about programming.

 

Thad** if Mastercam did not compensate for .500” to the left – then reverse the poles – I’ll never understand programming.

If it compensates to the left by .127 or .867, then this is not a simple 2D solution. This is a surfacing condition, solid model, or dimensional method of cutting with all three axis.

 

When we measure the 1” diameter cutter, we simply put 1.000 into offset D01 – some controls require half.

We cannot measure the actual dia, and then use a mathematical process to come up with the theoretical diameter at some certain depth – operators are not usually engineers, you’re lucky if they can perform simple trigonometry problems let alone know how to correctly read a measuring instrument.

We simply treat the radii, bulls, & chamfers as natural occurrences; this way we all remain sane!

Surfacing will calculate these things for us given the unusual shapes of our cutters – but only when we are not using a basic 2D profile.

 

Regards, Jack

[Jack Mitchell]

Sorry,

 

I missed the line Y-1.0 in the previous post.

 

Regards, Jack

[McRae]

Thad,

 

Strenuous day, re-read today and find I was indeed reading too much into the post. Are you in agreement with the rest of the posts though??

 

Confirmation that Contour will not do what you are asking.

 

[ 08-27-2002, 08:09 AM: Message edited by: MfgEng ]

[Thad]

Andrew,

 

quote:

---

Strenuous day, re-read today and find I was indeed reading too much into the post. Are you in agreement with the rest of the posts though??

---

I'm in agreement that it can't be cut dimensionally correct by using a simple pocketing cycle.

 

quote:

---

Confirmation that Contour will not do what you are asking.

---

I'm using pocketing, not contouring. But if I were to use a contour to finish the walls of the same pocket with the same cutter, it still would not cut to the dimensions of the pocket. MC compensates for the diameter of the tool, not the actual cutting diameter at finish depth.

 

There is still something that this forum is not understanding, so I'll try one more time. If I have a bullnose tool with a .250 corner radius, the tool will not cut a 1" wide slot until I'm at least .250 deep. Agree? Therefore, if I cut a pocket (or slot) that is not AT LEAST the corner radius deep, then MC is not cutting the pocket (or slot) dimensionally correct, because MC compensates for the dia of the tool (1.0), not the actual cutting diameter at finish depth (.867 dia at .08 deep).

 

I shouldn't need to use a surface pocket toolpath and I shouldn't need to use any additional toolpaths to machine this pocket. This is as basic as you can get. I want to cut a 3" square pocket that is .08 deep. I don't want sharp corners in the bottom of the pocket so I'll use ANY bullnose cutter. The radius size does not matter. Whatever is on the tool will be fine. I happen to have one that is 1" dia and it has .250 corner radius. I cut the pocket and measure it. The finished pocket measures smaller than 3" square. Why? Because when compensating for the diameter of the tool, MC respected the diameter of the tool, not the diameter of the actual cutting diameter. I don't know how else I can explain it.

 

gstephens workaround will cut the pocket too big. The pocket floor will be the correct size, but the overall pocket dimensions (radiused "wall") will be bigger. Scribe the pocket and then cut it if you don't believe me.

 

I believe this is a shortcoming in MC. Is this a glitch or am I expecting too much?

 

Thad

 

[ 08-27-2002, 09:41 AM: Message edited by: thad ]

[Thad]

gstephens,

 

I don't have the time or the energy to get into a pissing contest with you. Thank you for your input.

 

Thad

 

[ 08-27-2002, 09:39 AM: Message edited by: thad ]

[McRae]

I missused teh word contour - I indeed used a pocketing routine and came to the same conclusion. I do not share the opinion that this is a Glitch or error on the part of the software. If the feature that you describe is what you need then use the solutions provided. Because the software doesn't interpret the part as you want it to does not render it ineffective or Buggy.

 

If the purpose of the post is a functionallity request for "Axial" compensation then fantastic, lets push the limits for this.

[Guest CNC Apps Guy 1]

I'm with the others here. It's not a glitch. You need to use a surface toolpath. If you'd liek to have that functionality resident in the 2D Pocket toolpath, you'll need to send in a request to [email protected]. What you are requesting requires 3-D Compensation and Pocket only offers 2-D.

 

JM2C

[McRae]

BING-BING-BING

 

What about Constant Surface Speed for milling? This would be a fuction of the cutter diameter at the given depth of cut - Works for ball nose cutters and bull nose cutters and updates for each cut as it may change when surfaceing.

 

Think that thru...