Which type of tool profile to use to add a roundover point bit in ESTLCAM 12.x?

[Mattman (Matt K)]

I have a new roundover point bit like this one:

I’m not sure which profile I need to define this bit within ESTLCAM 12.x:

Do I use a ‘profiling tool’ profile to define it?
Or do I use the ‘tool with radius’ and put in a negative radius?
Anyone tried to do this with this type of bit?

[CesarH (cesar)]

I have done some fluted panels using ths type but used it as profiles bits running along the vector (just inported the straight lines (calculated the fluted form from sketchup)

[Tokoloshe (Philipp)]

These are my settings for a 2mm roundover endmill. There is a tutorial by Christian from Estlcam where he explains how it works. I set the height lower and the diameter a little bigger so that I would not have some edges if the wood is a little off.

[Mattman (Matt K)]

Thanks to you both. Profile tool it will be and then testing/playing with it to fine tune the dimensions and the measurements.

[Mattman (Matt K)]

Philipp I’m looking for that tutorial and haven’t found it yet. I only know how to say cookies please in German . If you come across it, please post. I’ll still look since what I did, didn’t seem correct.

I think I found it, is it this one:
Detailed view of tool list

It helped a little. I’m guessing EstlCAM doesn’t care about the radius and leaves that up to me to determine how deep to go as Cesar does/said. If so then I think I get it and will need to experiment with it.

[Tokoloshe (Philipp)]

This one:

It’s about a V-endmill, but the general idea is the same.

[Mattman (Matt K)]

Ok. I’ll have to watch and read the subtitles a few more times and then it should sink in my head. Thanks

[Mattman (Matt K)]

I’m not so sure this was the solution.
Here are some screen shots and results:
The tool setup/profile:

Then I did a test to just do a line with a depth of 5.1 mm and ESTLCAM shows it is going to cut down to the 7mm depth (which is what I set the height of the profile to, not the cut depth).

The cut was made down to 7mm, not what I wanted.
Seems I have to set the cutting depth to be the same as the height of the tool profile.
This is with version 12.155A. before I go for the upgrade, does version 13.x fix this?

[dalrun (Dave L)]

Yes, with v12 Profile tools there doesn’t seem to be any way around Estlcam cutting the profile as configured, e.g. depth = that Height: 7, any Depth or offset setting is ignored. To use 5.1 you’d have to set Height: 5.1 and Dia 2: 2.5 (6.35 - 5.1 = 1.25r x 2).

I setup profile bits as regular milling tools. To cut a full profile, Depth = profile height and profile width is entered as a negative Finishing allowance/offset (works w/ holes, parts and R/L engraving). For that 1/4" roundover: D 6.2 and Fa -6.2 (.15 less than max 6.35) is a safe max, D 5.1 and Fa -5.1 is also fine. For balanced profiles the Finishing allowance/offset is always the negative inverse of Depth.

FWIW, 90deg V-bit chamfering can be done the same way: tool diameter / 4 + chamfer width / 2 = D and -Fa, e.g. (4 tool / 4 =) 1 + (1 cham / 2 =) .5 = 1.5 D and -1.5 Fa.