V25 - How to Spiral

I've learned that if I have a round pocket and I choose the "Advanced Pocket" pattern and check "Adaptive Roughing", it will do a spiral (Mill 2-axis).

Here's exactly what I'm trying to do:
First drill a 3.5" hole. Then use a 1" end mill to drop into the hole and open it up to a 5" diameter.

I would choose "mill 2-axis"-->"Profile" and use the 5" diameter circle as my geometry, but I don't think there's a way to spiral when doing a "profile".
I think it has to be a "pocket", but it will start in the middle and sit there cutting air for a while. To eliminate this, I would select both the 5" circle, and the 3.5" circle as my geometry so that I will actually be in material. I would try to make the start point in the middle of the circle so that it will drop down where I have already drilled.

But the problem is that my 1" end mill doesn't fit inside the geometry, so BobCAD won't let me do it.
I have also noticed that when doing "Adaptive Roughing", it completely ignores what I select as a start point.
Being able to spiral is really really nice, but it seems inflexible.

Is this something like you are talking about.Note:I did not set feeds,speeds,etc.Just used defaults.
You can adjust easily how much width of cut and how many passes you take,,and also a finish pass if you desire.Also can pick climb or conventional cut and DOC.

If you can make a 3d model, I would start by drilling the 3.5 inch hole using a point on center of the hole. I would put a 1.5" diameter (or slightly smaller) circle on center of the hole, then use that as the internal boundary and a 5" diameter circle as the outside diameter to run a 3d slice spiral feature between the boundaries on the 3d model, leaving a small allowance for a cleanup pass. The 3d spiral will just end as a spiral, so the allowance will vary when it's done. Then I'd run profile feature on the 5" hole to clean out the allowance as a finishing pass.

I think you could do all of this on a 2d drawing as well by putting a surface beneath the drawing at the depth of the pocket for the spiral to run on, so you don't really even need a "model".

3D splice Spiral , followed by a Profile to open up a pocket from 3.500 inches to 5 inches ? I must be missing something.

I think he meant to "rough" open the 5" hole using the Slice Spiral, then run a finishing Profile. I hadn't fiddled with Slice Spiral much before, but playing with the settings gave me this, which I think does about what MJFILION had in mind, using mmoe's idea. I'm a router guy, not a machinist, so feeds & speeds are whatever they defaulted to, and thus wrong. :)

If I understand it, he wants to drill a 3.5" hole, then use a horizontal spiral motion with a 1" endmill to clear out the hole to 5" without cutting any more air in the middle than necessary. If that's the case, after the hole is drilled, you can use 3d slice spiral to spiral outward from inside the 3.5" hole to the 5" circle on a horizontal plane. It doesn't do a cleanup pass, so does not make a circle (it kinda just ends when it hits the set allowance distance and doesn't continue around at that amount), but a profile at the end can clean it up. It can be used like a spiral pocket routine, which is what I thought he was asking about.

It is only a 2 pass cut.Or maybe I am ass umming too much here.But a 1 inch cutter to me means a machine and set-up worthy of using such.There is only .75 a wall to machine.I also had ass umed this was wood or thin plate aluminum,,as he said he was drilling 3.5 inch cut.Maybe I am looking to hard into this.

I assumed the other way, that since he stated he's using an endmill and didn't call it a router bit, it is most likely steel or aluminum. Most router guys don't seem to call their bits endmills unless they are more into the aluminum end of things. If it's anything else, I don't think I'd bother drilling a hole first. I also was guessing that the material might be very thick, like 3/4 inch. Otherwise, like you say there really isn't any need to spiral at all.

3.5 diameter hole,there goes another thing I was ass umming,,and that would be a hole saw on thin plate.If he is actually using a drii bit and drilling a deep hole,,,,he gots a worthy machine alright.Maybe op can chime in.


3/4 inch is shallow to me.I do totally agree with the statement of why bother drilling at all.It is a simple pocket,,start to finish.Ramp in and go.

I'd call 3/4" steel or aluminum thick, and they would require a hole or a helical spiral into the material before cutting, but for wood or plastic it is certainly just plunge and go. :)

MJFILION,you being new to BoB,here is a link with a lot of info to help out http://www.cnczone.com/forums/bobcad...formation.html

Thanks for the responses guys. This is a 2-1/2" thick steel plate. Sometimes it's a through hole, and sometimes it's a flat-bottom hole.
I'm not a machinist, so sometimes I'm unfamiliar with nomenclature, so please forgive me.
I've been using BobCAD for a year and a half; we started with V24.

jrmach: In your first post you are correct with what I'm trying to accomplish. That is exactly how we used to do it - but I'm trying to spiral without "stepping" out.
Our parts are so simple that I haven't really played with any 3d machining before, but it looks like the 3D slice spiral is the ticket.

Trotline: That's it. I just had to modify the lead in so that the end mill would drop down inside the hole that we drilled instead of plunging into material.

Thanks guys.

Sooo,you ARE drilling a 3 1/2 hole ? Most impressive machine,no doubt.One place I worked many years ago we had a drill press that we could do that with,,needless to say,it was Huge.

Yes, it's a big machine. We're a fab. company and 90% of what we machine is 1"-3" thick structural steel plate.
It's our only machine, and we don't do anything that you would consider "3D", so I've never gotten around to exploring these features in BobCAD.

Hartford/Mighty Viper V2100
w/Mitsubishi M625 control

OIC,,now I see where your coming from.I was ass umming too many things from your fist post.Certainly not the norm for this forum.

MJFILION

you might want to try a profile of the 5 in circle
contour Ramping
set depth of pass at .125 to .250 max , until you see what your tool likes
your feed rate comes from the Z
get this set right you can punch some holes with method
make sure the slug has some where to go

If he has a big a** machine,and drilling 2 1/2 deep,I think that is the way to go.It really is incredible to see a drill bit cut a 3 1/2 inch hole thru 2 1/2 inch steel plate.I've done similar,I would c-drill,then 1/2 drill,then straight to 3 1/2 inch drill bit.64 rpm or so.


OTOH,,something similar to what dwood is suggesting might be worth trying.If you can mill 1/2 down,like dwood is suggesting,flip part over and mill just shy of 1/2 way.That way you do not have to mill near as deep,you can use smaller EM and you don't have to worry about the slug.After you mill second side take it out of machine and mini sledge the slug out.Put back and machine a finish pass.If you can get that to work,it certainly would be the fastest.This would be like Trepanning in a Lathe.This will take some doing to get everything to efficiently work right.

For what it's worth, when you use 3d slice to do this sort of spiral motion, you will need a model that has a bottom to the hole, even if it's supposed to be a through hole. I tried my suggestion of just using a surface beneath 2d geometry, but that doesn't seem to work with 3d slice. You need to model the part in 3d, but if it's 2 1/2" thick, you should add a 1/2" bottom so that the slice has a face to run on. Here's an example (V24, but you should be able to open it):

https://files.secureserver.net/0sA7gv6kd6dBAn

You also need to set the top of job to 1mm below the top surface of the part in the 3d slice feature, otherwise it will try to cut the top surface as well. Use the extract edges feature to get the outside diameter, then offset the circle geometry to the appropriate sizes. I used a slightly smaller circle for the outer boundary to keep the spiral from touching the finished surface. If you try to use the allowance setting in 3d slice, it also creates a bottom allowance, so you kinda have to make the allowance manually with the boundary. The finish pass then takes care of the rest. I did not pay any attention to feeds/speeds, so it's just an example.