Modeling question

[adze_cnc]

As you have surmised the tapered ball-end cutter wouldn't touch the sides so there's really no need to use it beyond the model's edge. Cutting the vertical sides is what square-end cutter and a profile toolpath is good for.

[zaxis]

. I used a .25 tapered ballnose to cut out this profile. I am happy with it, but wondering why my radius on the top and bottom ended up having this ledge. The profile I designed was tangent to the top and bottom surfaces making it a smooth transition??

[adze_cnc]

Have you ever typed something and thought "this is wrong—I think". What really should have said was you don't need to go down the sides. Sometimes going over the edge ( model boundary greater than 0 ) is a good thing as the above cut shows.

The following image show a 1/4" ball-end bit (straight sides) in yellow. The model cut is in blue. The solid white line is the surface. The dashed vertical grey line shows the edge of the model ( if you set boundary offset to 0 ),

Model boundary = 0 :

--

Notice the little curled up area under the bit centre?

Model boundary = 0.120 (just under the bit radius):

--

That curled up part cut away.

[zaxis]

In an earlier post I described the .125 offset and what the result was. The bit tried to plunge to the full thickness of the material on the first cut. I was air cutting because I was not sure about the result so there was no harm done. That is why I took out the offset for the finish cut. I did use a .25 offset in the roughing cut. I will reprogram that offset and try again....maybe I had something wrong. Thanks for the advice it makes perfect sense.......So I did give it a try and with the same result. I think it would work ok with a standard ball nose, however, being a tapered bit, it rubs when the bit plunges down the sides. ??

[adze_cnc]

You mentioned a 1/4" tapered ball nose bit. Is that a 1/4" diameter shank or a 1/4" diameter tip? If the tip is less than 1/4" diameter then 0.125 will be too much and cause spill over.

Setting the "Model Boundary" at 1/2 the tip diameter seems like a good place to set it to avoid "going over the edge" but due to software rounding errors there can be a few times when it does go over the edge—hence my choice of 0.120 above. Even that might be too much. I might then try 0.080 then 0.100 then maybe 0.090, etc. to dial in the amount by checking the toolpath display on the 3D view.

--

Model Boundary = 0.120" with a 1/4" dia ball-end cutter (not quite small enough to prevent spill over)

[zaxis]

#46294
Specification
(a°) Angle 0.10°
(D) Diameter 1/4
(R) Radius 1/8
(B) Cutting Height 1-1/2
(d) Shank 1/4
Overall Length (L) 3
Type Ball Nose, ZrN
Flutes 2
I tried several offsets down to .08 and still get a little ledge, maybe my design or software issues ....no worries it really is just a small cosmetic thing. I'm still getting the overall results that I want. Thanks again for nursing me along on this. I really get it now thanks to you.

[adze_cnc]

I presume that bit is from Amana? It looks like their part number and I found one on their site. It seems to me that I've come across this before and had a good laugh. To my mind it's really not a tapered ball-nose bit. I'd enter it as a plain ball-nose bit and save VCarve or Aspire the hassle of doing the trigonometry.

Let's pretend that this 0.10 degree tapered bit comes to a point and not a ball end. How long would the tapered portion have to be to come to a point? At 1/4" shank diameter the bit would need to be 71.62 inches long — 6 foot 1 and 5/8 inches. Add a shank length to fit in a collet and it's about as tall as me (a perfect bit for forum user "highpockets"?) .

At 1.5 inch cutting length what's the difference in diameter between the 1/4" shank and the ball end? 5/1000" (0.0052) or about the thickness of a branded yellow sticky note.

I can only imagine that they call it a 0.1 degree taper for legal reasons. I imagine some said "you told me this bit had a 0.250 inches diameter tip. But it's only 0.245 inches. I cut a really expensive piece of material thinking it was 0.250 inches and now it's ruined. Wait until you hear from my lawyer".

[adze_cnc]

EDIT: for some reason I have a problem with 71 inches. It is, of course, 5 foot 11. This not the first time I’ve made this confusion.

[zaxis]

I am attempting to use some of the installed clip art, specifically the Flourish 101-20-x or Flourish 101-11-x to create a border for a box lid. Is there a way to use the Flourish 101-20-x by sizing it up to a specific length and width? ie. 10x7.5. Not having any luck there I tried to extrude the 101-11 on a centerline rail but I get round corners and I need square corners. So I am at a loss to figure this one out on my own.

[zaxis]

OK....... so no one seems to be familiar with that question so ii put together my own design.....I have created a panel using the modeling tools in Aspire. First, I created the border using a center line sweep to the dimensions that I wanted. Next I created the center raised panel using a 2 rail sweep. The result is what I was trying to achieve. (not sure if the correct procedure was followed) The screen shots are shown below. Doing the rough and finish tool paths seem to calculate way too much time (used REST). I chose a .125 end mill for roughing and a .25 tapered ball nose followed by a.125 tapered ball nose to finish. This seems to be the problem. The finish tool paths are going over the entire surface and not just the perimeter and the small cove for the raised panel. I should be able to carve just the molded edges of my panel and leave the center flat without any machining on it. The error must be in modeling. I have not run yet because of the length of time on what should be a fairly short job. I'm new to Aspire....been using Pro for quite some time. Can anyone help?

[adze_cnc]

As a VCarve user I'd cut that using the moulding toolpath. But others may have better Aspire ideas.

...and a .25 tapered ball nose followed by a.125 tapered ball nose to finish.

Are the sizes quoted shank size or the ball's diameter / radius? If shank size then the latter is more informative.

[zaxis]

The sizes are ball diameter....

[zaxis]

As a VCarve user I'd cut that using the moulding toolpath. But others may have better Aspire ideas.

...and a .25 tapered ball nose followed by a.125 tapered ball nose to finish.

Are the sizes quoted shank size or the ball's diameter / radius? If shank size then the latter is more informative.

Thank you Adze, The answer is molding toolpath. Sometimes I can't see the forest for the trees!!

[zaxis]

Success!!! Thank you all for helping me out learning how to only "begin" to use Aspire. I am thankful for the forum and folks willing to help out a newby. What I set out to do in my imagination is now a reality. All that is left is stain and finish