new Agie user with questions

I'm learning to run an Agie Classic S and have a few questions. First, I'm cutting a die detail with land and taper. It started off by cutting the taper followed my skimming the taper cut. I didn't mean to skim the taper but it did and another thing I need to figure out. After this it went on to the next detail which is a dowel hole. I don't see anywhere on the piece details screen where it's going to go back and cut the land. Will it go back and where do I look that shows me this? Secondly, when the machine starts to cut it takes off slow. I'm guessing this is normal as the Charmilles I use to run did the same. However, with the Agie it will get about a 1/4 of the way around a .500 dia. hole before the power kicks up and cuts with balls. Can this distance be changed anywhere so as it kicks in sooner?
Thanks all.

I assuming the Classic has the Vision control. It did a skim cut because of the technology you chose for the surface finish. When you select the technology from the options it gives you, it tells you how many trims cuts it takes for each available technology setting.

I guess the hole is a machining in your piece? What order the machine cuts stuff is dependent on the strategy you selected. Right click on the piece and then you should see an option for strategy. It can get a bit confusing with all the options but the simple options are if you select early, it will do the main cuts on all the on the machinings, wait for you to do the separation cuts and then do all the trim cuts. If you select late it will do all main and trim cuts up to the separation point and then wait for you to fix and remove the slugs.



The soft start and exit are to ease the wire in to and out of the job, When defining your machining on the entry tab there is an option called entry -> contour this is the length of the soft start, and on the exit tab the option Contour -> exit this controls the length of the soft exit.

two things. it sounds like you just only added taper to the machining.you need to use the collar workmodel it will create 2 machinings in a workgroup 1 for land and 1 for taper with 2 different quality targets. Don't pick add machining, pick add machining from a group workmodel and pick collar. 2nd always do at least 1 trim on the taper. this is particularly important for draft angles less than 1 degree. lastly in machining details>entry you will find a parameter labled "entry->contour" this value will determine where the machine will switch from entry tec to main cut. 0.000 is where the lead out meets the contour. A positive value will move the point onto the contour a negative value will move the point down the lead out line. hope this helps. D'oh, Steve is that you?