Trouble defining Ogee bit

[Rcnewcomb]

I'm trying to define a CMT 848.817.11 as a form tool. It's not obvious to me what is wrong with the vector so I'm asking others to point out the issue. See the attached EPS file along with two pictures.

[LittleGreyMan]

Randall,

You have a negative slope at the bottom of your vector. Editing the second node solves the problem.

[sharkcutup]

Try putting the profile in the proper orientation for CNC operation as in image above.

Be sure to get the dimensions correct when creating profile.


Sharkcutup

[Rcnewcomb]

Yes the curves were off and I just did not see it.

Got it defined now.

Mischief managed.

Thanks!

[redwood]

First off, I never thought I would see the day when Randall would need help. He is a supreme giver of help.

Second, from my past life, I have tons of edge forming router bits that I've never thought to use in my CNC. Is there a tutorial somewhere that shows how to set up these bits and add them to the tool database.

[LittleGreyMan]

First off, I never thought I would see the day when Randall would need help. He is a supreme giver of help.

I guess Randall was so tired playing with his new toy he simply couldn't clearly see his screen anymore.

Second, from my past life, I have tons of edge forming router bits that I've never thought to use in my CNC. Is there a tutorial somewhere that shows how to set up these bits and add them to the tool database.

Er, tough question. Something like a manual perhaps

See "Adding your own custom form cutters" in the manual or the help file. Or ask Randall

[LittleGreyMan]

BTW, I'm pretty proud to be THE guy who helped Randall. It just made my day.

Thanks for noticing.

Code: Select all

Repeat
 (-;  
Until pigs will fly

[Rcnewcomb]

Code: Select all

BTW, I'm pretty proud to be THE guy who helped Randall.

LGM,
Over the years I've learned that sometimes I can be too close to the problem and "know too much" to see what is blindly obvious to someone else.

In this particular case I was too "clever" for my own good because I was using arcs instead of Bezier curves. With the arc it wasn't obvious that I was forming an undercut. I never thought about converting to Bezier until I saw your response.


Adding your own custom form cutters
Before opening the tool database, draw to exact scale the Right side of the cutter geometry in the 2D Window Use the Node Editing tools to create the arcs and curves etc.
Only draw the Right-hand side of the cutter geometry to the correct size and scale as shown in the image above.

The shape can be a combination of Lines, Arcs and Bezier spans, but the shape cannot have an undercut such as a dovetail bit. i.e. starting at the bottom the vector must go up and/or to the right -- never down and never to the left.

With the vector Selected open the Tool Database (using the command icon on Toolpaths tab or from the main menu, Toolpaths ► Tool Database In the Tool Database window, click New... Select Form Tool

The selected geometry will be imported and a profile displayed in the window.Give the Cutter a meaningful name and enter the cutting parameters - speeds and feeds etc. Click the Apply button to save the new cutter into the database list so it can be used at any time.

Note: Cutter geometry can be imported as dxf, eps files and used to create Form Tools in the database.

Can I create a tool with an undercut?
No, the Form Tool will not allow a bit with an undercut to be modeled since toolpaths using bits with undercuts cannot be previewed.

If you need to use a bit with undercut in a project, you can create a toolpath using a standard bit but run that at your machine with the undercut bit installed.

For example, you want to create a T-slot using a T-slot bit. You can create a toolpath using an end mill and preview that, realizing at your machine there will be a horizontal slot cut at the bottom of the toolpath. To do this safely and successfully, you need to have a good understanding of toolpaths, how to set up a single pass toolpath and possibly the use of Lead-ins and Lead-outs.

If you need help setting up a particular toolpath, asking on the Vectric Forum should get you the help you need.

[CrowsWW]

Some manufacturers have a DXF for the profile all you have to do is ask them and they will send it to you for FREE!