Custom Tools onto Curved Surfaces ( again )

[Superman]

G'day all, Help required on custom tools in X2. they are not working out the same as in V9.1

 

In V9 I had success with custom tools (on or near to) touching curving surfaces But for the life of me I can't get any tools to do what I tell them to in X2 ( not so strange an event).

 

I'm using same comps and tool settings used in V9

and have tried:-

- undefined tool with custom profile ( drawn full size )

- endmill / ballnose / bullnose with custom profile ( drawn at scale that Toolrad = 1.0 )

 

I have drawn tools correctly ( frmm 0,0,0 in X+Y+ quadrant, no c'line, chains OK, no duplicates, on it's own level, and so on..) also tried having tools embedded in the current MCAM file, and as they all display OK in backplot and verify. So this is not the problem area

 

------ but bugger me ---- it still won't *@!#% work

 

I am having problems loading my package to the FTP site ( under construction )

 

as usual it's a job required Yesterday ( 1 week ago )

 

Any input is welcome

 

Thanks all in anticipation

[Guest CNC Apps Guy 1]

I've had trouble with custom tools that have splines in them. Use lines and arcs only and more than likely you'll be in good shape.

 

HTH

[iowajim62]

Have you tried importing your V9 Tool Library ? Just wondering if those tools would cause the same problem ?

[Superman]

Thanks for the quick repy

 

Tool profiles are only lines and arcs ( splines not used in any profile to eliminate problems.)

 

I had a quick attempt in V9 again, I am getting same result now as in X2 ( not good )

 

Last resort will be doing the t/paths with standard profile tooling ( facemills, ball bullnose - all on steroids )

 

Tools I want to use are "ISCAR FEEDMILLS" and special finishing tools to increase stepovers ie. 12mm endmill with R12.0 ground on the face with R1.0 corner fillet ( sorry guys - we're metric down-under )

Picture a 24mm ballnose, now grind the flute OD to 12mm diameter and break the corner with R1.0 ( this is my finish tool )

[iowajim62]

Another question, do you have the "As Defined" box checked in Backplot and Verify ?

[Superman]

Tool is showing itself correctly in backplot and verify and our systems are set to show tools "as defined"

 

this toolpath is set for cutting in a 3-axis machine setup before passing onto a 5-axis machine for swarfing and holes

 

PX this is an "aero" part so I can't play with it at all.

[gcode]

Steve,

 

I recently had trouble with a custom tool

in X3.

The solution was very simple..

All I had to do was draw a horizontal line

from the top of the tool to X0

 

I am using a custom tool def for an Iscar feed mill and its worked OK for me though I have not done any difficult 3D work with it.

[Leigh @ Kodiak]

I'm just curious...

 

 

If the tool shows fine in backplot and verify, what exactly IS the problem?

[Superman]

gcode- the tool profiles all start at X0 Y0 and chain to finish at the X0 line

 

Problem is that the form of the tool when stock allowance on drive and check surfaces are set to zero, the tool is stil a loong way off the part ( even more if I have allowances )

 

It appears as if a bullnose cutter is being used when a ballnose is the tool

 

Picture a cylinder ( side view ), the tool would touch only at the quadrant points ( top and sides )

[gcode]

are you setting the radius of the tool in the

radius field.. I've found this neccessary with custom tools

[Mike Whitten CAD/CAM Contractors]

Hello Steve and all,

 

As far as I have studied in the past, what Steve is trying to do is impossible in Mastercam.

 

Mastercam will not and have never been able to comp to a Custom Tool shape. It is possible quite often to find a spot on a Standard Tool type to comp to and then create custom tool geometry that is scaled so that it will still comp and also backplot and verify correctly.

 

If you use an Undefined tool type, it will simply comp to the diameter that is input on the tool definition. It is represented by the yellow line.

 

Mastercam Help explains this:

-----------------

Custom tool profiles and tool profile geometry (Mill/Router)

A tool profile is geometry that describes the shape of a tool. Mastercam uses the tool profile to simulate a tool in Backplot and Verify. Mastercam provides a tool profile for each tool type shown in the Tool tab of the Define Tool dialog box. These tool profiles are stored in separate Mastercam files in the MCAMXMillTOOLS or MCAMXRouterTOOLS directory. For example, the file FACEMILL.MCX stores the default tool profile used by all face mill tools.

 

Mastercam provides a variety of tool types, each with a corresponding default tool profile. When you define a tool using one of Mastercam’s built-in tool types, Mastercam automatically scales the default profile based on the tool diameter and other dimension that you enter in the tool definition. This ensures that cutter compensation is displayed correctly in Backplot and Verify.

 

You can customize tool profiles in either of two ways:

 

You can edit (or replace) the standard profiles, just by opening them up in Mastercam

 

You can create entirely new ones with the Undefined tool type. Use this technique when you need to use a tool that does not match any of the standard tool types. On the Tool Type tab, choose the Undefined button.

 

 

For the Undefined tool type, Mastercam calculates cutter compensation based on the diameter that you enter in the Tool tab. When Mastercam previews the user-defined profile of an Undefined tool in the Define Tool dialog box, the compensation point is indicated by a dotted yellow line on the profile as shown below.

 

 

When you backplot or verify an operation using an undefined tool with a diameter that differs from the custom tool profile, the geometry in the custom profile does not match the cutter compensation, so the tool will appear to be offset from the part.

 

To display a custom tool profile during simulation, select the As defined option in the Profile section of the Backplot options dialog box and the Verify options dialog box.

 

You can save the custom tool profile geometry in either a separate Mastercam file (like the standard tool profiles) or on a level in the part file. An advantage of saving a custom profile to a level of the part file is that the tool geometry can travel with the part file if it gets moved to a different computer. When saved as a separate Mastercam file, the file will need to be moved along with the part file and placed in the same location on the new computer as the old computer.

-------------

 

HTH,

 

Mike

[Mike Whitten CAD/CAM Contractors]

Steve,

 

I just had a look at the shape of the Feed Mill insert. The only issue I see is the small radius. If you are are only cutting on the large radius, a bull mill standard tool type with a scaled custom form may work. I have done this in past and it has worked for me. You must scale the bull mill at the full diameter though. In other words, the OD of the custom tool will not measure 1 unit(mm in your case) as the outside of the tool is not really there.

 

Mike

[Superman]

Michael, Hi

 

Thanks for your comfirmation that the standard way won't work.

The newer "ISCAR" feedmills, I have changed my attack to having them as facemills, as for the older ones, they will have to go as bullmills

 

ie,

standard feedmill OD 20mm with base dia. of 6mm and main radius of 11mm

is defined as 'bullmill' OD = 28mm, corner rad =11mm ( custom shape, I agree, will have to be played with, and **note** it is only a representation not the actual cutting shape)

** As to verifying your tool and path - check against a STL model in verify **

 

The special finishing tool I'm using ( 12mm OD with R12 nose ) is now done with 24mm ballnose, just have to modify my boundries.

 

This is one that will have to go thru "VERICUT"

 

Thank You Michael and All

Steve

[Mike Whitten CAD/CAM Contractors]

Hello Steve,

 

It sounds like you are on the right track. It may be a good idea to drag the cutter through a piece of scrap material and measure the profile with a cmm or comparator. You can then be sure of the actual cutting profile. I would also do a STL compare in Mastercam or Vericut, Vericut would be best.