17+ hours to cut a strip of molding... any advice on bits?

[skintigh]

I'm replicating a "classic cove and bead" molding that is about 3 inches tall, 1.5" thick, 48" long, and I'm cutting 2 of them out of a 48" white pine 2x8. (I'll then chop them up and use them as dentil details) My bit selection is limited, so I started by choosing a 1/4" end mill for clearing and a 1/8" tapered ball nose, but that was going to take 17+ hours according to Vcarve. Clearing with the 1/4" end mill didn't save much time at all.

Then I got the idea to rotate the molding so all the carving was right at the face of the wood. I would carve the face, then use a table saw to cut the back and side of the molding. But that would still take 2+ hours (in a makerspace that's only open for a few hours).

Is that a reasonable time? I watched a few videos on molding but they didn't discuss bits or cut time.

There is a 1/2" end mill I could maybe use for a clearing pass, but I couldn't find any numbers for using it with softwood, and I've never used a straight bit before. It's an Onsrud 48-072. https://www.onsrud.com/Products/48072.asp

Should I use that? Should I buy a different round nose bit or other bit you suggest? Thanks!

[steve_g]

What cutting strategy are you using?
SG

[steve_g]

Hopefully you’re using the Vectric moulding toolpath tool… if not, here’s a synopsis of how to…
https://drive.google.com/file/d/1jQjl9pxKUuY5x3A9zncAF-GAvXkm6Vps/view?usp=sharing

[skintigh]

I'm using the molding tool path. Tried with and without a clearing pass.

That presentation is enlightening. So he's saying I should skip a clearing pass, just use a 1/8 ball end, and cut the full length of the bit at once as long as I ramp in? That certainly sounds faster than cutting 1/8" deep per pass! I will change my design to do that tonight.

That fluting info is also very interesting. I tried a fluting tool path on an unrelated project and found it to be utterly useless as I didn't happen to own a bit the exact width and exact depth of the flute I wanted. I ended up making a molding profile and path for the flute I needed. Looks like there's a way I could have used the fluting path by stacking a bazillion flutes, but how did he make all those vectors? Is that an array copy or is there some tool to do that? Looks very powerful!

[Brady Watson]

What are you running for CAD/CAM?

[skintigh]

What are you running for CAD/CAM?

I'm using Vcarve pro (free trial and makerspace editions) and a ShopBot Buddy.

[steve_g]

That presentation is one that I did for the Austin Texas Camp ShopBot last year… The “slides” went along with the presentation and may suffer some from not being live!

Yes… I cut moldings without a clearing toolpath IF the cut starts at the surface and proceeds with a very low stepover percentage. I’d most likely recommend an 1/8” tapered bit.

The bazillion lines to cut fluting paths with are rapidly done with copy, past, rotate… repeat!

Feel free to ask further questions either here or as a PM!

SG

[skintigh]

Thanks for the info and presentation!

So I made a new bit and entered the stats for the 1/8 tapered bit, including a cutting depth of 1.5 inches, saved, and... now Vetric has completely deleted that setting...?!?!? It's just gone. Not the number, the entire box where you type the number is gone, as is the label for that box. That can't be normal.

Anyway, I see no way to set cut depth in the molding path, in tool settings, or editing the tool itself. I tried watching the animation to tell how deep it's cutting but it wasn't helpful.

It seems to be faster though, down to 15 hours.

[steve_g]

Would you mind posting your profile vector? When I do a rudimentary bead and cove 3” tall and 48” long, my estimated time is 1.5 hours. That’s cutting with a tapered 1/8” bit @3IPS and 4.5% stepover.
SG

[bob_reda]

You are quite limited with the trial version of the software, a lot of things do not work for obvious reasons.

[skintigh]

Ok I think I attached it.

[steve_g]

http://www.talkshopbot.com/forum/attachment.php?attachmentid=32199&stc=1

Well… I guess that’s that!
SG

[steve_g]

I don’t imagine that the trial version will let you export the vector as a DXF either… if you can, take a picture of the vector or a cross section of the actual molding, and I’ll redraw it!
SG

[skintigh]

Doh! It's the makerspace version so I thought I could share it, but maybe I can only share it with the same makerspace version. That would make sense...

Here is a screenshot of the molding profile (actually a pair, slightly altered as the original is thicker than a 2x8) and the settings. The path is a straight line 46" long. Onsrud taperd 1/8" bit 1.5" CL. With the current settings the molding pass takes 5:32:59 with rapid rate 100 scale factor 1. I have no idea what to set those last 2 to.

3220232203

[scottp55]

Aah, Just looking at some recent putzing of 3D's.
Lion's were done at 4% stepover, and then 6% stepover with a Chinese .25mmR TBN..and I CAN'T tell the difference.
Also a recent project with accurate multiplier for estimates with the same bit(but at 1.5,1.5, and 6% stepover..so multiplier should be close.
Maybe go at least 6% stepover, and use a multiplier of 2?
Not any experience with Moulding Toolpath Yet, but should be even higher multiplier I think?
scott

Listen to Steve though!
Oh Steve..Those little .25" depth and CA'd "Twig Butterflies" kept my Aunt's 5/4 Black Walnut cracks from spreading.. this pic was 2 years later, and the flatness of he board after 2 years curled almost .5".
I put that down though, to having those "Butterflies" on both faces, and almost the same spots. Just mentioning after 2 years.

[srwtlc]

Try a 8% to 10% stepover. 3% is way to small. If 10% leaves too much sanding to clean up, then drop it down further. Don't trust the calculated machine time. Run one with optimal settings and then tweak the scale factor to match the actual time that it took. After that, you can use that scale factor for similar toolpaths.

Try it without/with 'vary stepover' enabled.

Don't put your kerf line in there, as the bit will take more time to drop in at that spot and if it fits, it could drop all the way down and make a full depth pass.

[skintigh]

I set the speed to 4 IPS pretty much randomly. The ShopBot speed sheets recommend 1.8-3 IPS and cutting 1xD. But I'm cutting up to 12xD but with only a 6% step over, so can I go faster? Even full speed -- 6 IPS?

It's an $86 bit so I don't want to take any big risks... But if I start at the most shallow cut and maybe make that square trench in the middle super shallow it will be safe?

[steve_g]

I eliminated the down cut separator between the two moldings and would plan to separate them on the table saw, it would have to eventually be cut there anyway…

It’s my understanding that the reason you need a multiplier for the time is that the Z action time isn’t calculated into the mess. This tool path has VERY LITTLE Z action… just a slight step at the end of every 46” of travel. I have found that no correction factor is needed when cutting moldings.

I’m seeing 2:28 total time for both moldings.

SG

http://www.talkshopbot.com/forum/attachment.php?attachmentid=32206&stc=1

http://www.talkshopbot.com/forum/attachment.php?attachmentid=32207&stc=1

[skintigh]

That's great, thank you! So you think I should stick to 3 IPS? What step over percentage did you use?

I'm going to try running this today.

[steve_g]

My stepover of 4.5% will result in almost no sanding… at least in MDF, likely your SPF also. If some sanding is ok, move it up to 6% or so.

My machine would like to run this at 3 ips yours may be different! My machine is getting up in age and needs some TLC! If yours is new and tight, bump it up!

SG

[skintigh]

I made the center trench about 1/32 deep. I tried 4% and 4 IPS, it was so slow I could die.

So I started over at 4% and 6 IPS. (I wanted to stay low on the step over just to not stress the bit.) Anyway, the estimate is 2:49. That seems close, right now I'd estimate at least 2:18. I may stop it half way through unless I can find something else to do while babysitting the machine. And/or flip it around and start it using a higher step over.

Thanks everyone!

[srwtlc]

If you have a bunch of these to do and don't want to have to do a roughing pass, but would still like to have some material removed to relieve some stress on the tool and you, you could do multiple passes on the table saw with a dado blade to remove the bulk of the material. You could even do an angled pass over the blade to make a concave cut that came close the the profile. If you have an alpha, you could run 4-6ips, but may sacrifice some quality the faster you go.

I do a lot of 3D designs, and using 8%, I have little to no sanding with 1/8" and 1/16" ballnose tools (just fuzzies). The downstep or steepness of parts of your profile may dictate that though.

[coryatjohn]

Maybe I'm crazy but it looks like 95% of that molding could be done with a 1 1/2" round nose and a 1/2 end mill. The only part that's 3D is the curve at the top and that could be done easily with a sander. Round nose bits are tough and cheap.
32208
($26 on Amazon)

[skintigh]

I think my estimate was optimistic...

I looked into router bits but could only figure out how to do half of it. But the longer I sit here the more I question doing it this way. I could 3d carve some sanding blocks and use those and table saw or router to make the molding. The sanding might be faster than this.

The fastest way would be to 2D cut them but I'd need a longer bit. Might be worth it depending on how many of these I end up making. I think I shouldn't need much more than 4' or 8' strips, but the fiancee tends to like to add details as the project gets closer to completion.

[Brian Harnett]

A roundover bit and cove bit in a router table would make easy work for that, sometimes the old ways are faster. CNC is a tool not an end all machine.