Inventables Community Forum

More Depth and Better Finish - help

HI,

I’m using 1/8 straight bit this modal.
But to cut through these pieces is taking me a lot of time.
The chip size is too small and dusty, with recommended settings on easel.(with 1/8 straight bit)
I have to cut 10 pieces of the same modal.

Need help in selecting the bit which cuts through more finer and with more depth for every pass.

Ideally the project that i work are 2d (cutting though the wood), or stencils.

Thanks

The depth of cut seems to be extremely shallow

Hi @PhillipLunsford

The depth per pass is 1mm.

@Prashanth Can you give more detail on your settings or share the Fusion project? If you’re getting dust, you’re feed is too slow, your router speed is too fast or you’re cutting MDF. An upcut bit will do a better job clearing chips.

Hi @NeilFerreri1

The settings and bit that i used.
Material - Hard Wood (Rubber Wood)
Bit - 2F Straight End Mill - 1/8" - Black
Feed Rate - 1016 mm/Min
Plunge Rate - 304.8 mm/Min
Depth Per Pass - 1mm
Spindle Speed - 3 ( around 21k RPM)

Fusion Project link : https://a360.co/2GBCGoy
(forgive me which the project, im trying this out for the first time)

I will try upcut bit.

The carving took almost 40mins.
I wanted to try more Depth Per Pass, was scared if i would break my bit.
(Its hard to find the bits in india, i have to order it from inventables)

How do i cut though the material faster and with more finer edges.

Thank You

i’d slow the router speed down to 1. and try an upcut.

1 Like

Slotting is the most difficult operation because the endmill is mostly engaged and it’s difficult to evacuate the chips. Turn the router speed to one until you get into much higher feeds. I’d think the stepper motor will lose steps before a 1/8" endmill would break. Make sure to ramp the cut and you can double your plunge rate. Use the feed override to increase the feed while cutting until you’re no longer comfortable and then back it down a bit. I’d also go a little deeper to start, say 1.2mm.

1 Like

Hi @NeilFerreri1

I dont have any upcut bits with me know.
i have "Solid Carbide - Fishtail Spiral, Upcut Bits- 1/8 in " which are ideal for plastic.
Can i use it for wood?

Or should i go ahead with 1/8 Straight bit? i will follow the above suggested settings.

Thanks

The fishtail should be fine. They are pretty good for thin plastic, but you have to make sure your stock is well secured with any upcut bit. Anyway, like I said, I’d go with the upcut for slotting in solid hardwood. The straight bit will have to work harder because of the chips. You may not break the bit, but you can ruin them by rubbing away material rather than cutting it.
For what it’s worth, if your goal is speed, get a bigger bit. You could always come back and clean up with the 1/8" if you cut most with a 1/4".

1 Like

Thanks @NeilFerreri1

Will get back with results. :slight_smile:

My X-Carve has been upgraded a lot since its purchase but the general idea should still apply to your ( vanilla? ) one.

Below is a picture of my Microsoft Surface Dial’s Delrin Transport Case I made a few weeks ago:

Before cutting the chamfer, the vertical surface had a total length of 19mm which is close to 3x the diameter of the ONSRUD 52-080 ¼" 2F UpCut Endmill I used to do like 90% of the OPs on the shell.

In order to get this, IMHO, really nice finish I split that particular OP up into 4 parts:

  1. Four 2.375mm cuts to half the 19mm full depth with 2 Multiple Finishing Passes of 0.66mm, Finish only at final Depth and 0.25mm Radial Stock to leave - So 4 cuts at 2.375mm each and the 5th cut at 9.5mm.
  2. Two clearance cuts to half the depth with 1.5mm Radial Stock to leave.
  3. Four additional 2.375mm cuts starting at half the 19mm full depth to full depth with 2 Multiple Finishing Passes of 0.66mm, Finish only at final Depth and 0.25mm Radial Stock to leave - Again 4 cuts at 2.375mm each and the 5th cut at 9.5mm.
  4. One final cut at 19mm full depth with zero Radial Stock to leave but a Repeat Finishing Pass at 1/3 the feed rate.

Here’s a short Video visualizing it ( Step 2 Clearance Cut not shown ):

Alternatively, you could also model a channel and use an Adaptive Clearing OP to clear it out which would allow for cutting depths of 1½-2 Tool Diameters ( or more ) at once.

1 Like

Hi @durahl,

Thanks for this, would try this weekend.
been waiting for bits to arrive.
will update you about my project very soon.

Thanks