[dcutler35]

I am trying to chamfer a hole with a chamfer mill e45 d.5-w.75 the hole is 1.875 diameter hole for a 2-8 un-2B the problem is I have forty holes and I was told I have to select each hole as a contour? this is problematic because it is a solid model and selecting each holes takes forever. any suggestions greatly appreciated.

[txcncman]

I am assuming you are using Toolpath > Contour. Why not window your selections? If needed, put them on a separate level and turn the other levels off. If they are in a rectangular array, you can do one then Transform that operation to the locations.

[dcutler35]

that sounds like a good Idea also i am going about .010 on my chamfer over the major diameter and down a little moe than than the chamfer is that about right?

[txcncman]

I assume you will use 2D Chamfer. If your tool is defined correctly, follow the prompts in the setting parameters.

[seijack]

When working with solid models and you need to select many holes of the same size.. you can create wire frame that you can select all at once by using this method... Create > Curve > Curve on all edges...using this method you can create selectable wire frame geometry that you can select..you can do this for the whole object or just one surface..piece of cake..

[Superman]

#1 - change all the core diameters to a new color or level
#2 - set your filter mask ( upper toolbar ) ( not the ALL button ) & set the check on for that color or level you did in #1
#3 - select the 2D contour op, then when asked for the chains, select the window icon that is shown on the chaining dialog box
#4 - window select the entire display, and accept-- it will then ask for a start search point ( this is where you want the operation to start from )
#5 - the operation parameters will then open for you to set what you want to do-the chamfer amount will be about 0.085" to give a finish diameter of 2.050", you want the tip to project about 0.040" past the lowest point of the chamfer. With these settings, the NC code should have a Z-0.125 while actually cutting the chamfer

----make sure you have defined the tool correctly & accurately, the important data for a chamfer tool is the base diameter & the angle, E45 D0.5 W0.75 --- I'd say the base dia is 0.50", @ 45° with a 3/4" shank, the OD and flute depth is not critical but should be reasonably close

[dcutler35]

superman if i am pulling holes with a major diameter from a solid model cant I just set my step over to .010 and then put my tip offset .05 ?

[Superman]

superman if i am pulling holes with a major diameter from a solid model cant I just set my step over to .010 and then put my tip offset .05 ?

I assume by step-over, you are meaning the chamfer size ?

Yes, as long as the geometry you select is the intersection of the hole with the top face. Those numbers would give a chamfer that is Ø0.020" than the selected geometry

Now, if the chamfer is already drawn on the solid model, you would typically set a chamfer size of 0.001, & the tip offset to be 0.050 deeper than the largest sized chamfer that your op is to machine. ( your chamfer would be 0.002" oversize, on some jobs it may be critical, your choice, adjust geometry, or adjust tool lengths or tool comps
ie you have a 0.010" & a 0.050" chamfer drawn, you pick the top face geometry, set chamfer size =0.001", tip offset=0.100" (0.05+0.05)

A 3D chamfer would also work along the same lines