Create a new form tool

[khaos]

So there I was trying to create a tool that is basically a sphere on a stick. Aspire thinks I'm daft and I don't know why it will not allow more than the bottom half of the tool...

So given this I am sure that Aspire has no ability to undercut. That is to come in from the side of a cut and create a ledge.


Can anyone help with this?
4206 Shouldn't everything in the red box be vector to create the form tool?

[tmerrill]

Joe,
You are correct that Aspire/VCP/Partworks does not show an undercut or allow you to generate a tool like you show. There was a discussion on the Vectric forum some time ago where Tony explained why. That discussion was specifically about using a keyhole bit, but the same applies here.

By using the Lead IN/Lead OUT feature on a profile toolpath you may be able to do what you want. It would have to be a single pass type toolpath and you would have to adjust your depth calculation to be to the center of your bit. Hope this makes sense.

Tim

[Gary Campbell]

Joe...
You can use and toolpath an undercut bit. You will not be able to define or draw it as it actually is. You may want to call it a ballnose of the correct diameter. Since you cant define it accurately, you wont get an accurate preview.

It is most likely that you will have to hand code the leadins/outs to make sure that you do not get any unwanted retracts.

We use the same strategy for keyhole bits. They are usually hand coded and retracted in the same location they went in.
Gary

[tmerrill]

Gary,

What do you mean by hand coding?

I use Aspire to make keyhole slots frequently and simply draw a line that doubles back on itself. For accuracy I normally do that by manually entering the X,Y coordinates of the three points. Once Aspire generates the toolpath I don't have to touch the code.

For Joe's situation the built-in Lead in and out options should work fine.

Tim

[butch]

I do keyholes and undercuts regularly. But I always hand code the file. I lay out a line and that gives me the X and Y measurments. I then go into edit and just make a file to drill in and return to the same spot before retracting the Z.
I do this for keyholes with keyhole bits, Finger pockets in drawer faces with a finger hole bit, undercut edges with dovetail and roundover bits. It's not hard, just have to make certain that the bit Z down is in a clear area, then brought to the cutting position then pulled back to a clear area before retracting.

'
'For ShopBot Control: SB3 Alpha
'
'Keyhole for pocket on top/Z=top, 1/4 keyhole bit/Set router RPM to 12000
PAUSE
'Header that shows up on screen at start of file run
'Turning router ON
SO,1,1
PAUSE,2
'
MS,1.0,0.5
JZ,1.5
J2,0.000000,0.000000
J3,4.75,7.5,1.5
' Bring to start of hole cut
M3,4.75,7.5,-0.35
' Drop into the board to start keyhole cut
M3,4.75,7.85,-0.35
'Move .35 inch to form keyhole
M3,4.75,7.5,-0.35
'Return to start
J3,4.75,7.5,1.50
'Retract from hole start by moving Z above board
JZ,3.0
SO,1,0
' Turn spindle off
J2,6.000,30.000
' Park clear of work area

I find this is much faster and more accurate than drawing two lines and having it cut up and back. I had too many Z moves in unexpected spots.

Butch

[tmerrill]

Thanks Butch for taking the time to provide such a detailed answer.

I've manually programmed before when I only had Partwizard, but haven't seen the need since I started using the Vectric products. Other than a rapid plunge a couple of weeks ago with 3.6.3, I haven't seen any unexpected Z moves.

What I did is create a library of Keyhole files. I mostly do horizontal ones and depending on the size of the project, I have a 1", 2" and a 3". For vertical I just have a 3/4". I simply use a laser positioner to put the bit over the center and run the size I want. They could easily be made into custom files, but I haven't done that yet.

Tim

[bill_moore]

I was looking for a way to cut keyholes when my search brought me here. I do not know anything about coding so I tried some of my own ideas. I draw a circle the diamiter of the entire keyhole I want. Then I go to node edit and make a start point at the point of the circle where I want the bit to enter and exit. Then I grab one side of the circle and compress it to a circle .01 wide. Toolpath it as a profile cut on the vector using a start point. It works great. This is the low tech version. LOL