Creating User Defined tools

[Kel61]

Hi Guys.

 

I'm having trouble creating a user defined tool using a sketch or file for that matter.

 

The tool is a double angle 45 deg cutter mounted on a sub arbour. Attached is a .jpg of the cutter created in Solidworks.

 

We use MasterCam for Solidworks.

 

Any thoughts?

 

regards

 

Wayne.

[Dtm]

Hi Guys.

 

I'm having trouble creating a user defined tool using a sketch or file for that matter.

 

The tool is a double angle 45 deg cutter mounted on a sub arbour. Attached is a .jpg of the cutter created in Solidworks.

 

We use MasterCam for Solidworks.

 

Any thoughts?

 

regards

 

Wayne.

 

 

In mastercam you must only draw 1/2 of the tool. I always draw the right side, but I'm not sure if it matters. There also must not be any other geometry on the level. When you select undefined tool select the level your geometry is on.

[gcode]

In regular Mastercam, the defining sketch must bt drawn in Top plane.

Try making the profile sketch in the same plane as the Top plane of your MCfSW session

[Kel61]

In regular Mastercam, the defining sketch must bt drawn in Top plane.

Try making the profile sketch in the same palne at the Top plane of you MCfSW session

 

Tried doing that and to no avail.

[Brando]

i have reg mastercam, i seem to remember having an issue similar, i think i drew a small radius where the 2 angles met (on your tool od), and that fixed the problem

[gcode]

See the attached SW sketch.

In my test file it was labeled as Sketch 11

In the undefined tool definition I selected Sketch 11 and the tool came in OK.

I also tried to make the origin the tip of the dovetail and that did not work so I will submit that to QC

custom tool.PDF

[Scott Lundin Shopware Inc.]

gcode,

How do save the file? As an sldprt in the mill tools folder? Can the tool be saved on a level within the sldprt for the workpiece like in standalone mastercam? More details please.

[gcode]

The sketch was a standalone sketch in the sldprt file.

The undefined tool parameters page has a Sketch dropdown and all the unused sketches inthe file show up.

When I revolved the sketch into a solid, it disappeared from the dropdown and the tool definition went dirty

I haven't tried it as a filename yet

[gcode]

OK... when you revolve the sketch and make a solid from it, it closed the sketch... and that wrecks the sketch as a tool definition

I deleted the solid, but the tool was still dirty ... I had to open the sketch and the the line SW entered to close the sketch.

Then the tool definition was valid again

[gcode]

It looks like undefined tools only support MCX-6 files if you want to

use a file to define an undefined tool.

I have an extensive library of tools like this from regular MC and have used them often in MCfSW

and never thought about it.

 

MCX-6 is the only option available in the file dropdown.

I tried saving the sketch as an sldprt file and selecting that using "all files" but the definition failed.

It looks like a sketch in your working file is the only way to define a custom tool if you don't have regular Mastercam

[Ryan Butt CNC Software]

Hi guys,

 

The trick to remember with custom tools in MCfSW is the geometry all needs to be in the positive quadrant. Y+, X+.

 

Take a look at the attached image. In the left side image you'll notice we have some tool geometry in Y- as well as the center line. This is the geometry causing the problem. Smart dimensions in - are fine)

 

To correct this we just need to delete the ".25" dim, add a coincident relationship between the origin and the lower left of the tool, and shift the center line into +. Now the tool can be defined.

[Scott Lundin Shopware Inc.]

Thanks guys. I got hung on this a while back.

[Ryan Butt CNC Software]

gcode brought up a good point, in standard Mastercam you can define a custom tool with geometry in Y- and users do find it useful. So I submitted an enhancement request to get this added to MCfSW - cnc00108363

[gcode]

Thanks

[Kel61]

Where does the sketch have to be saved to?

 

Does the sketch need to be open when creating the form tool? Is the sketch saved as a solid part?

[gcode]

the sketch needs to be in the same file as the Mastercam ops are running in.

the sketch needs to be a half profile of the tool with a contruction line as centerline..

if you close the sketch and use it to make a revolved solid, it will not work as a custom tool definition

 

it also needs to be drawn in the Mastercam Top plane

[Ryan Butt CNC Software]

"it also needs to be drawn in the Mastercam Top plane"

 

Actually that restriction only applies to standard Mastercam. In MCfSW we can draw and use custom tool geometry on any plane. This is great when working in assemblies.

[gcode]

Thanks, I'll have to try that