[Spooq]

Hi,

can anyone tell me how to define a fly-cutter in Sprut 7?

Thanks!

[keebler303]

A large diameter cutter with 1 flute?

Seems pretty easy huh?

[Spooq]

Sounds very simple but... if I set z-step to 0, then Sprut crashes. And if I set max plunge angle to 0, then it seems to change all my tools to that.

I'm sure this is simpler than I am making it. Do I just need to make sure I only select waterline operations that start outside the workpiece?

[keebler303]

I've never used sprutcam! I would think your Z step should be the max depth per pass rather than 0. There should be an option for "do not plunge" but maybe there isn't?

Good Luck
Matt

[mike sr1]

Sounds very simple but... if I set z-step to 0, then Sprut crashes. And if I set max plunge angle to 0, then it seems to change all my tools to that.

I'm sure this is simpler than I am making it. Do I just need to make sure I only select waterline operations that start outside the workpiece?

The bottom level should be a a negative number, less than zero, that determines the depth of cut.

Post your file, as there isnt any information to go on as to what you are trying to do..

[Spooq]

Looks like I won't be able to post anything for a while I will try to come back to this in a couple of weeks, sorry.

[dbrija]

The bottom level should be a a negative number, less than zero, that determines the depth of cut.

Post your file, as there isnt any information to go on as to what you are trying to do..

I have had this same experience. It would seem like I could define bottom=0 and still generate a toolpath. I just set the bottom level to -.00001 and its happy....

[mike sr1]

I have had this same experience. It would seem like I could define bottom=0 and still generate a toolpath. I just set the bottom level to -.00001 and its happy....

I usually set the top level to "0"
The bottom level to a negative number, say -.010, and it would take .010 off the top of the part if using a flycutter.
When I locate center in the model tab it sets the z to 0 on top of the part and it defines the bottom level as per the drawing (negative figure in the bottom level box) greyed out, in waterline or flatland finishing parameters tab.

I may not be doing it correctly either but it works for me, the bottom level numbers are always negative numbers.

[arich]

to setup a fly cutter in SC you start by making a big end mill with one tooth. I have found there is no simple way to tell SC not to plunge a tool, you just have to setup the operation so that plunging doesn't happen. The best workaround I have found is to use waterline roughing, set lead-in/lead-out to tangent, then under strategy set machining strategy to parallel (not equidistant which sometimes plunges). Depth of cut should never be zero, you set that to the amount of material you want to fly cut off in each pass. Bottom level should be whatever face you are fly cutting down to. Remember - waterline roughing and finishing will not mill into your model, so make sure your workpiece is defined with some material above the top of the model or it won't let you cut anything.

Alternatively you can draw 2d geometry representing the path you want the fly cutter to follow and use 2d contouring to cut along these paths. Be careful w/ this though, it is a dumb operation and will let you mill into your model. It will exactly follow the contours you specify in a series of passes from top level to bottom level, and each pass cuts at the cut depth you specify.

[mike sr1]

[QUOTE=arich;1207849]to setup a fly cutter in SC you start by making a big end mill with one tooth. I have found there is no simple way to tell SC not to plunge a tool, you just have to setup the operation so that plunging doesn't happen.

In feeds and speeds, the approach can be set to a percentage of the work feed so that the tool plunges to the new depth at the percentage you have set in approach feed.

[arich]

That changes the feed rate at which your tool approaches the workpiece, not the plunge depth. There is also a plunge feed rate setting, again though, that only changes the feed rate not the fact that the tool is plunging into the work.

I was saying there is no direct way to tell SC to only approach from the side with a tool like a fly cutter or other side cutter. The roughing waterline - parallel method works and 2d contouring are the only ways I have seen to ensure side cutting only.

[mike sr1]

That changes the feed rate at which your tool approaches the workpiece, not the plunge depth. There is also a plunge feed rate setting, again though, that only changes the feed rate not the fact that the tool is plunging into the work.

I was saying there is no direct way to tell SC to only approach from the side with a tool like a fly cutter or other side cutter. The roughing waterline - parallel method works and 2d contouring are the only ways I have seen to ensure side cutting only.

You are correct. I misunderstood what you were trying to do.

If I am going to fly cut the top of a part I have been doing it with mdi, set the z to the depth I want, zero x then enter the feedrate and how far I want x to travel. I just use this for facing off the surface before I start the program.

[arich]

I concur, fly cutting is often not worth the trouble of programming with SC, manual gcode entry is much faster.

[Spooq]

That changes the feed rate at which your tool approaches the workpiece, not the plunge depth. There is also a plunge feed rate setting, again though, that only changes the feed rate not the fact that the tool is plunging into the work.

I was saying there is no direct way to tell SC to only approach from the side with a tool like a fly cutter or other side cutter. The roughing waterline - parallel method works and 2d contouring are the only ways I have seen to ensure side cutting only.

Thanks Arich, this is the info I was after.