Sprutcam drill point compensation and spiral plunge help

[Tbkahuna]

I am a new Sprutcam 7 user. I have been building models in Alibre and exporting as IGES files. There are two things I can't seem to find.

Drill point compensation - I don't know if that is the correct term, but here is my issue. I am trying to drill a .25" diamter hole to the depth of 1.115" as it is designed in my model. I end up with a hole where the tip of the drill is 1.115", but the .25" diameter section is only 1.042" deep. It looks to be because the drill tip is at the depth of the model. I have tried changing the "tooling" point and "contact" point for the tool as well as making the bottom level deeper. It always maxes out at that level.

The second is for getting a spiral plunge during Hole Machining. I am trying to cut a .5" diameter hole .75" deep using a 3/8" carbide end mill in 1018 steel. I know the tool doesn't have much clearance, so I thought that by using a strategy of spiralling at 100%D with a .031" deep step would take the tool down without a 90 degree plunge. The cut is only .031" also. Maybe is ok to plunge 90 degrees, but I like a ramped plunge until I get more comfortable with the Tormach 1100. I have done a similar cut when clearing a plane, and it just didn't sound/look right, so I am trying something different. It appears to cut ok in the simulation, but on the machine it appears to do a direct 90 degree plunge when running the program to cut in the air. It is at 80 fpm and 3.3 ipm for a 4 flute carbide end mill.

Can anyone give me advice on doing a spiral plunge (for various roughing and finishing) strategies and also on plunging a 1/2" end mill at 90 degrees for up to .062" in steel?

Thanks for any help.

[saabaero]

Doesn't seem as my previous post took so let me try again...

Drill point compensation - Pick the "Hole machining" operation and select the holes. In the (left) lower window click "Job assignment" (the 2nd button from the left - depicted as a cross section through a bore) select the hole to modify and press the "Properties" button above. When the "Hole editing" popup window appears, from the drop-down under "Drill tip compensation" select "Drill tip". The hole depth will then be compensated based on the drill point angle to provide a full diameter hole to the depth in the model.

Spiral Plunge - Pick the"Hole machining " operation, select the "parameter tab" then select "strategy". Under the "Drilling type" dropdown select "By spiral". Or you can do a 2D contouring operation and under Parameters\Stretegy select "Helical machining".

I always prefer to pre-drill holes and pockets as in the long run it saves time, extends the life of costly endmills, and just seems easier on the machine. Drilling is always the least costly and fastest way to remove material.

[saabaero]

OH! And forgot to mention that certain machining operations allow for spiral or zigzag plunge under "Parameters", "Lead In\Lead Out".

[Tbkahuna]

Thanks for the help. I am making progress!!