PDA

View Full Version : Helical Pocketing

jdingus
09-14-2008, 09:11 PM
When performing helical boring in surfcam.
i.e. taking a 2" Indexing mill and helically interpolating down the center of the
bore to rough it out. Ideally would like to do a finish pass at the bottom of a blind bore.

Know of a few ways just wanted to know quickest / easiest you guys have came across, seems like there should be a more direct way to perform.

1) 2 axis pocket - set helical plunge - play with parameters to where the plunge is in the center of the bore

2) Draw helix and then 3 axis contour

3) True Mill - heard this way but don't know the settings to use

Judge Leo
09-15-2008, 09:46 AM
Option 1 should give you the results you're looking for. By getting the job done in one operation you can save the operation and re-use it later.

jdingus
09-15-2008, 09:58 AM
Do you happen to know how to change the parameters so it ends up going down the center of the bore?

When you set it to helical plunge and the defaults it normally helically plunges down the sidewall and then finished the bore at the bottom.

By changing the parameters we can get it close but haven't figured out the exact way to do it. It's always off by a couple thou or so.

thanks,

jd

tnik
09-18-2008, 08:50 AM
yea, its pretty simple.. I'll walk ya through it..

first, when you select the geometry for the contour path, make sure you pick the center as the plunge.

then say you have a 3.5 bore - 2.0 deep to do, and you pick the top geometry of the hole, in the Z depth and stepdown , put 2.0 , then choose the helical plunge.

angle can be left at auto

radius: set to constant and use this formula

radius of hole - radius of cutter - stock you want to leave

eg. 1.75-1.-.015 = .735

I ususally leave min width at default

then you just play with the pitch number to get the ramp angle/pitch that you want.

setup your finish pass like normal, and your set to go..

hth ;)

jdingus
09-18-2008, 09:47 AM
Exactly what I was looking for.
Been playing with some other variables that I think was messing me up.
Will try this out.

Thanks again

JD:rainfro:

Titaniumboy
03-08-2013, 12:13 PM
yea, its pretty simple.. I'll walk ya through it..

first, when you select the geometry for the contour path, make sure you pick the center as the plunge.

then say you have a 3.5 bore - 2.0 deep to do, and you pick the top geometry of the hole, in the Z depth and stepdown , put 2.0 , then choose the helical plunge.

angle can be left at auto

radius: set to constant and use this formula

radius of hole - radius of cutter - stock you want to leave

eg. 1.75-1.-.015 = .735

I ususally leave min width at default

then you just play with the pitch number to get the ramp angle/pitch that you want.

setup your finish pass like normal, and your set to go..

hth ;)

I'm taking a Surfcam class and I was surprised when the instructor had us make helix geometry in order to do helical boring of a hole. I would have thought this was pretty elementary stuff in CAM software?

The procedure up above (thanks tnik!!) comes pretty close to generating the tool path that I want. The only problem is that the toolpath, after helixing down to depth, insists on moving to the center of the hole before doing the final cleanup pass at depth.

For thinner material this toolpath might be acceptable, but the problem I'm working on now has us cutting a 6" diameter hole out of 2" thick material with a 1" diameter endmill. Thus the Surfcam toolpath would have the 1" endmill traveling almost 3" from the edge of the hole back to the hole center at the full depth of 2".(chair) There is no way I or the instructor is going to find this toolpath acceptable.

Am I stuck creating a helix and bottom hole geometry to create an acceptable helical hole bore?

Titaniumboy

moldcore
03-08-2013, 05:21 PM
Not sure if you’re trying to pocket the entire 2” or just want run a contour around the 6” hole until it breaks thru. In V6 they have added the ability to ramp down the inside of the hole.

Here’s the video:
2-Axis: Contour Ramping (http://www.surfware.com/surfcam_tutorials/2_axis_contour_ramping.aspx)

Markced
04-04-2013, 07:59 AM
Helical plunge boring can be done with no guess work at all. I have been doing it for years with excellent results. there are a few things that are very important to make it work properly.

This example is for helical boring a counter bore or thru hole to size on the first pass. Once you understand how it works you can make adjustments for leaving stock to finish if needed.

First select geometry, (it must be circle or combination of arcs that make a 360 degree circle). Then before selecting "done" select "plunge" then "center" then the same geometry you are machining, (you should see the pick reference snap to the center of the circle) then "done". When selecting tool its best if you can use a tool that the diameter is at least as big or bigger than the radius of the bore to machine.

If the tool dia. is larger than the rad. of the bore than on the cut control page set all the parameters for the side cuts to "0".
Set the Z depth parameter to the disired depth, and make sure the Z ruff depth is set to the same amount. "0" finish cuts, and "0" stock to leave in Z.

Set the Plunge to Helical and set all the parameters to constant. Make sure plunge clearance is set to "0".
If it is easy math to figure out the helical radius you can plug that in now. In case of a bore size that is some number not evenly rounded off, it is easrier to just accept the default and generate the tool path now.

After generating tool path, look at the finish pass at the bottom of hole. Analyze the radius and copy paste that rad. into the helical plunge radius parameter and regenerate the tool path. You will now see that the plunge radius matches the fin. pass radius exactly. Remember this only works if the helical parameters are set to "constant".

At this point you can play with the pitch setting to get the ramp angle you want.

In the case of a larger bore radius that is bigger than the tool diameter you will have to make multiple helical plunges by setting the cut control to leave stock on the side, and adjust helical plunge radius to match the fin. radius of the tool path at the bottom of the bore as done above.

wjb1060
07-13-2013, 02:02 AM
I’ve always been disappointed that Surfcam hasn’t added helical milling as a choice for a stand- alone operation. I use an option that hasn’t been mentioned that I like and I use it all the time. This method makes a helical cut and finishes with a single pass at the bottom.

Demo: 1” bore with a 3/8 end mill, .75 deep. Pre-drill hole leaving 1/32 stock or more to be removed.

1. Mic your end mill accurately. Subtract the end mill diameter from the finished hole size.
1” - .374 =.626. Draw a .626 circle centered on the 1” circle (both at Z=0 for the demo).

2. Choose NC -> 2axis -> Groove Mill.
3. Chain the .626 circle and the Groove Mill Tool Information menu appears.
4. Fill in all the blanks as you normally would except make the feed rate and plunge rate the same because only the plunge rate value is used by the software for this operation.

5. Go to the Cut Control Menu.
6. Set the Grove Width to the finish hole size. This is only for your reference since the software will not use the value in this box to do any calculations.
7. Set the Groove Depth to the depth of your hole (In this case .75).
8. Set the “Geometry is The” to the center top radio button (middle spot on the top row). This causes the software to put the center of the end mill “on” the .626 circle that you drew.

9. Z Depth is: At Geometry.
10. Rapid Plane is: 1”.
11. Plunge clearance is: .1.
12. Change Plunge type to Ramp. This will open up the Ramp Angle box. Accept the default value of 7 for now. You will most likely be changing this value later.
13. Direction: Climb
14. Rough to: 0
15. Maximum Depth of Cut: Must be set to the Groove Depth value (.75) or it will cut in increments until the Groove Depth is reached.
16. Choose OK
17. Measure the distance between the coils of the helix in the front view (ctrl+2) and adjust your ramp angle to not overpower the axial clearances of your end mill and give a good finish.

Experiment with this method. It’s quick and very accurate. I have a new machine and I routinely cut my dowel holes with this method because I can ensure their location.