toolpath filtering quetion

[mike.b]

if you were to generate a toolpath on a surface and then filter it with a large tolerance...would all the toolpaths still be outside the surface, or would they take a 'shortcut' through the surface? i have no real apllication for this i was just wondering happy friday

[Thad]

I rarely filter toolpaths, but I would think that they would not violate the surface. The "corners" they would cut would be to leave you a little extra stock.

 

Thad

[crazy^millman]

Well to be honest this would matter on what advaned setting you set for the gaps. The filter is to use G2 and G3 moves in what planes you filter and keep the toolpath knitted to the surface during machining using the filter amounts you select there. I can have them as small as .001 and .0005 respectfully. It really boils down to the work you are doing if working on Foam models with a .75 endmill and a .05 step over then .01 would not really show up but if doing a .031 endmill with a .0005 step over and havea .01 then you may notice the edge look a little off and more faucted becuase it will then make no arc moves smaller than .01 becuase the filter is set to go no smaller than that. I find that filter cuts alot of our toolpath down in size fro 10 to 50% in size most time we use them and yeild much better results on surface finished and edge defintions in doing so.

 

HTH

[cadist]

I think I had a problem in past with filtering the toolpath with large tolerance. The corners got filleted in a very strange shape.

[Lee.]

You can check this by running a simple surface toolpath, saving the toolpath as geometry and then analyze it to see where it went.

 

HTH, Lee.

[Jim at Gentex]

quote:

---

I find that filter cuts alot of our toolpath down in size fro 10 to 50% in size most time we use them and yeild much better results on surface finished and edge defintions in doing so.

---

Good point. I also filter everything, but never w/ large tolerance settings. Another upside to filtering is usually a much shorter NC program, which saves run time.

[BernieT]

quote:

---

if you were to generate a toolpath on a surface and then filter it with a large tolerance...would all the toolpaths still be outside the surface, or would they take a 'shortcut' through the surface?

---

I'm sure the filtering process does not care where the surface is. It will take the 'shortcut' either above or below the surface but within the tolerance specified.

 

I like to use the filter whenever the toolpaths are in the G17, G18 or G19 planes; as Ron said, much smaller NC files. When using 'Constant scallop' or 'Radial', filtering doesn't do much good because the filter cannot make arcs in the above mentioned planes.

[Müřlıń®]

I have found this on filtering.

 

If you set your filter to .01 when you do a Surface/Rough/Pocket, you will get a much smoother flowing toolpathg without all the small arcs and lines.

 

Running a 1 1/2 feed mill @ 100 IPM will show this more readily than a ball.

 

With a filtering of .001(my normal setting), the toolpath stuttered around more because it had to follow all those small increments.

 

So leaving .03 stock usually mean no gouges.

 

 

Murlin

[Thad]

quote:

---

I'm sure the filtering process does not care where the surface is. It will take the 'shortcut' either above or below the surface but within the tolerance specified.

---

Bernie,

 

Someone isn't understanding something here...and it may be me. Just to clarify, what do you mean by "shortcut" and "above or below the surface?" I understood the 'shortcut' as the tool violating the surface because of a loose tolerance. I understood Mike saying 'outside' the surface, meaning not inside, or violating. You lost me on 'above or below.'

 

Thad teh clarification

[mike.b]

i think he meant below as inside and above as outside. i am going to try out lee's test. i think bertau has the answer..when mcam filters toolpaths the surface model isnt in the equation anymore so a large filter tolerance would violate the surface. thanks for the answer guys.

[Jayson Kramer]

I just ran in some trouble with a customer were I did not use Filtering on a rough pocket path made for a mold on a fadal.

 

With know filtering at all the machine errored out trying to run out the side of the machine.

there was a strange arc out put. but was fixed by filtering.

 

I usally use the filltering 98 percent of the time.

 

But this last one was a weird one.I thought it was there machine and they tried on two of them with the same result.

 

Took the program to another customer shop and began testing. to come tru with the results I did.

 

Short note:

Sent the code that was giving use and issue to Fadal and they did not find an issue.

 

JM2C

[BernieT]

What mike.b said pretty much covers what I meant.

 

I'm thinking vertical milling machine cutting 3D surface - above is 'outside' and below is 'inside' (ignoring possible vertical surface).

 

[TheePres]

I personally never use filtering on Fadals, seen some strange results at times. For other machines, i use half the surface profile call-out as my filtering tolerance. No specific reason, just out of habit.

[TKDBB]

with our Fadals, we filter but always uncheck the arc designations. We also have had the machine do strange and disaterous things if this is not done.

[Thad]

quote:

---

I'm thinking vertical milling machine cutting 3D surface - above is 'outside' and below is 'inside' (ignoring possible vertical surface).

---

DOH! It makes so much sense now. At the time I replied, I still had the situation in my Detect Flats thread in my head (vertical surfaces). I read your reply and I couldn't see the forest because all them damn trees were in the way.

 

Thad

[TS53]

If I understand how MC works, in the tolerance settings window there is a ratio variable. The fields are ratio, (off, 1:1, 2:1, 3:1 & custom), filter tolerance, cut tolerance & total tolerance. I think the ratio values will allow the surface to be violated up to the tolerance value. with a large tolerance there would be more violation than a small value. I usually use a total tolerance of no more than .0001 (but we produce high precision parts).

If I am off base, feel free to correct me.

 

Tim

[jctjct]

I have had rough toolpaths undercut the finish surface from using too high settimg in filter. I tightened up the filter from .005 to .001 and the undercuts went away.

[Thad]

I'm surprised that there is a "feature" that would make a toolpath violate the surfaces.

 

Thad

[Code_Breaker]

First, draw a circle. This is your goal. You want a circle. From each point to the next is a smooth transition. If you “filter” the circle “too much” or with too high of an amount, you can reduce the circle to a bunch of straight lines. Now, using point on the circle, draw a octagon, a hexagon, a pentagon, a square, a triangle, a straight line 180° from quadrant to quadrant. Each time you filter, you make less of the desire circle which you were looking to achieve.

 

One other thing, it imagine that you are running on a circular track. You stride is much smoother. If you take “shortcut” in one of the shapes previously mentioned, you have to slow down when coming into the corners and then try to pick up speed when leaving. The sharper the corners, the greater the distance you have to start to slow down.

 

This is what is taking place on a CNC machine, especially with a “look ahead” variable feed rate. I usually set my filter amounts on roughing to 25% of the amount of stock I am leaving, and 10% for semi finishing. For finishing, I use either .0001 or .0002, depending of the material. And, in all cases, I use 2 to 1 filtering ratio.

 

These are just my thoughts on the subject.

Hope this help

have fun

 

Code_Breaker

[crazy^millman]

I say try this on any machine that is over cutting into surface run the same part at 20 ipm and see if you have the same problem. This is the machine and by tighting up the tolerance you give the start and stop more of a place to get ot where as with it lose the machine say ok the transtion from point a to point b is great so I can haul a$$ to get there. Every machine will over cut if put in the right position so us to tool delfection accountability, Tool Wear, Machine Dynamics, and other Factors that come into play that might be causing these problem as mauch as you think filtering is. Ask code breaker said % do what you want and what you do all come into play and decide the final product as much as the code going to the machine.

 

Case in point we have a Fadal that was cutting parts off by as much as .005 at anythign above 20 ipm when did a PM on the machine and had ro rplace all the resolvers guess what it now cuts good at 100 ipm. PM and attention to the machien are just important as anything to make good part when is the last time it was calbrated or has it ever been done? Not trying to sound like an A$$ but al of this is just as important as filtering a toolpath is.