resolution,tooling or file?

[outcaststudios]

hello!
just recently completed one of my first very big cuts in urethane board.

in the preview in Vcarve the model looked ok , but after cutting its simply too ragged (see the attached picture. the circles need to be smooth and theyre not!). the good news is that the layout,strategy and material all worked great. i set the feed rate for 3.00 and the cutting took about 20 hours straight. i now know that i shoudl have set the feed for 6-8 ipm instead. so ...waht went wrong here? i used a 1/4 inch down cut bit for both the rough and finish. the resolution was set to 'high' the stepover was conservative at 10% and the pass depth was .125 (probably could have been .25 or more this stuff cuts like butter) also how can tell how long a cut will take in the software? i cant seem to find anything that tells me the overall cutting time? thanks!
-gregor

[knight_toolworks]

not sure what went wrong but if you had a bit with flutes long enough to cut full depth you could do this without the roughing pass in the foam.

[outcaststudios]

i thought as much, i was terrified so i went the conservative route. so the total depth of the deepest cut is 1 inch , what bit would you suggest i get?

[outcaststudios]

also woudl it be crazy to just attempt the entire cut with a 1/8 tapered ball nose and only specify a finish path? if so that would be great.

[knight_toolworks]

in foam usually it would not be a issue. I can't tell how big it is but could you use a 1/4" bullnose upcut? you can get them 2" of cut length. I have cut foam in one pass with them. what I do in a 3d cut full depth I will run one pass full depth slowly then stop the cut change the speed to what I want and then go for it. that way the first pass is where your removing a lot of material but after that the steps are much smaller.

[outcaststudios]

i will look into getting a 1/4 bullnose upcut , the total piece is about 48x40 and its 1 inch thick. the detail is super important. even with a ballnose 1/8 tapered bit specified in the preview in Vcarve, it still looks a little choppy...

[Kyle Stapleton]

Not trying to be a jerk, but what is it? The top part looks like you could do it with a 2d pocket around the nobs and then hit them with a vbit or a round over bit to get the edges right. As for the holes if it need two be smooth you will need some kind of bull nose bit.

6-8 ipm seems ungodly slow.

[outcaststudios]

kyle,

it is a .stl file from a model made in solidworks of a grate. i am importing the .stl and just running it from there. i could also do the entire thing with vectors but it seemed like a lot more work, plus i am a total beginner! the holes that pass through need to have 1.5º of draft on them,so they taper as they reach the surface. what speed woudl you suggest i cut at (6-8 woudl be slow i guess) also how do i get an idea of how long a cut takes? is there a function to tell you teh expected cutting time? thanks!

[Kyle Stapleton]

This is all 2d work, get the vectors.
I will post a video later in the day.
For the draft I would use one of these http://www.amanatool.com/catalog/category/view/id/723/?bcuttingheight=3155&filterable_angle=3357 the taper is only 1deg (don't think you will miss the .5 deg in foam) as for speed 2-4 ips is where I would go.

[Kyle Stapleton]

Hope this helps.
http://screencast.com/t/JDFDZMNMlI

[srwtlc]

One thing to look at would be the triangle/polygon count of your stl. It could be a low count and this would give you a surface that has many large facets. On top of that, if you scale it up, it could get worse. From your description, I'd say it would be better and faster to do it as a 2d cut or just a 3d cut around the bumps (whatever they are) and 2d for the rest. For the holes, a 1.5º 0.125" tapered ballnose would do the trick and by using a spiral ramp, it would be fast. For this toolpath, I'd set your rapid for the Z axis as fast as possible (standard or alpha will dictate how fast) and remove the dust foot. This way, when the toolpath for each hole is finished, it will rise up fast and without the dust foot, the waste piece won't 'jam' the tool. Doing it this way saves a lot of time by not having to pocket out the hole. For SB's, we generally use inches per second, so 3 ipm would be .05 ips, and that would be sloooow. Perhaps you meant ips.

Using a 0.25" downcut endmill will never give good results for finish toolpaths, as it needs a ballnose to follow the contour properly.


As Kyle demonstrated, just use the spiral down toolpath and let the waste piece stay or pop out and clean up later. Saves a lot of pocket time.

[outcaststudios]

WOW!! super super helpful guys!! ok i will head back to the drawing board and give it another go, i think kyle is right for sure ...2d is my friend here. the 3d was just more convenient at the time,due to my limited knowledge. wow!

[srwtlc]

There's also a ramp setting that will make the spiral down toolpath cut a bit faster/better, by keeping the machine in the set move speed and not dropping into ramp speed. I use this toolpath strategy to cut golf ball holes and by using the 1.5º tapered ballnose to cut it, the ball wedges nicely in the hole.

That ramp setting (VR) is Minimum Dist to Check and set it to .05 to make it a bit quicker. Set it back when finished to default of .15 or the better choice of .08.

[outcaststudios]

ok so it is definitely better to cut this 2D ...much better results. however the holes and the bumps are not round as they are supposed to be.
i checked the motors pinion to be sure it is fully engaged ,they are. the file was from DXF so i know the holes were round in the file. and the vectors were also round when i selected them in Vcarve...what else could be causing this? its on some but not all. i will post pics asap.....thanks!
-gregor

[srwtlc]

Gregor, take a close look at the circles by selecting them with 'Node Edit'. If they are true circles, you should see only 4 nodes and no extended handles. I'm guessing that since it was a dxf, that you'll see many, many nodes and this will make for a segmented or choppy circle that could also be out of round to a degree. It might be best to completely recreate the 'circle/dot' pattern with the drawing tools and copy array tools.

Post your dxf if it's ok to do so and we can take a look at it too.

[outcaststudios]

scott,
will do , i will do that asap.appreciate the help! the original file had fillets and draft added to it ,so there were definitely concentric circles in the dxf file ,which makes perfect sense since it would import all that information from the 3d model. thanks again!
-gregor

[outcaststudios]

here are two shots of the same piece. there seem to be different results throughout. the pocket operation that i did to get the round(seen here as almost hexagonal) bumps used a 1/4 straight cutter. shoudl i have used a different cutter? the master DXF file is forthcoming ...some of the bumps are round and others are hexagonal or just sloppy, why is that?

[ADAPT_Shop-Brady]

Have you ran the file in preview mode in SB3 to see how it appears there?
Might be helpful to upload your sbp file here to if possible for keen eyes to review.

[outcaststudios]

i tried to upload the dxf and the SB3 docs but they exceed the website limit. anywhere else i can post them?email? i did run a preview in vcarve and it looked a littel ragged too. not in sb3 yet im still trying to figure out how to do that in that program.

[outcaststudios]

here is a jpeg of the master file (dxf)

[Kyle Stapleton]

You can send me it in an email, just click on the woodworking link and and you will find y contact info at the bottom of the page and send away.

[srwtlc]

Do you have a OneDrive, Google Drive, DropBox account? You could try zipping the file up with a program like 7-zip (free) or win zip and that should compress it to be small enough. What is the file size?

Jpg doesn't really help any.

Bad vectors or a loose machine. Have you checked the grub screws holding the pinions on the motors? Not sure what you have for a machine. Older ones tended to loosen up and the shaft would turn inside the pinion.