Vericut Question

[gcode]

I'm running a toolpath with a Sandvik Ø2.5" button cutter

I want to slow the cutter down as it hits corners.

I'm  thinking  running Optipath chip thinning will give me what I want because there is more material in the corners

The tool is defined as a revolved DXF contour.

When I try to run Optipath it say chip thinning optimization is not supported with concave cutters

That doesn't make a bit of sense to me

I'm running 12mm inserts taking a .050" DOC so this is really a bull endmill despite being a button cutter

What am I missing ??

 

Is there a work around?  TIA

[?Mark]

Really strange that it thinks it's a concave cutter. I'm assuming that you checked the geo. Have you tried defining cutter manually? I have had trouble with using dxf on few occasions.

Just for kicks, adjust LOC of the tool to a little over .050 doc that you're running it at and see if it tricks it?

[Mick]

Try running it with a generic bullnose cutter (ie, a 2.5" diameter radius corner endmill) and see if you get the same error.

I would expect it is something to do with the DXF input.

[gcode]

6 hours ago, Mick said:

Try running it with a generic bullnose cutter (ie, a 2.5" diameter radius corner endmill) and see if you get the same error.

I tried this late yesterday afternoon and was able to get Optipath working with chip thinning

Chip thinning appears to be the correct approach.

Its slowing down coming into corners and speeding up coming out of them.

I told Optipath it cannot create new code and the federate changes are too abrupt .

I think I need to allow it to break the code up so it can decelerate into corners and accelerate out of them

I'm running a 14" gage length C5 Capto stack with a 63mm button cutter on the end and it DOES NOT like corners.

I'm hoping I can talk them into buying a  C5 Silent Arbor, but they run about $2K so there is not much chance of that

I'd feel a lot better if I could get Optipath chip thinning to run with an accurate representation of the tool though,

especially if I am going to allow it to modify the toolpath

 

[mkd]

what about the high feed function in MC? I've had luck with that slowing the corners.

 Also i watch the video on Vericut's new "Force" function. No experience wtih Optipath or "Force" but the new video is highly intriguing.

[gcode]

VC Force.pdfI rebuilt the tool using a Sandvik solid model and Optipath chip thinning is running with a properly defined tool now.

My seat of Vericut has the Force setup page in the tool definition and it does look intriguing.

I haven't tried it though. I think it's an option that must be purchased and the Force page is just eyecandy to lurie

you into pulling out your check book

\

see attached screen shot

 

 

 

 

 

 

 

VC Force.pdf

[Colin Gilchrist]

Force is really an awesome product, but it also requires you to buy a "proven" material/tool record. They test out a cutting tool based on 6 parameters, and use a dynometer to measure the forces the cutting tool experiences. Based on this, they are able to apply the physics based approach to improving the cutting. The main issue I've seen is that you have to buy a "tool/material" definition for anything you want to optimize. Say you are cutting Inco 625. You've got a 1" bull endmill with 40 degree helix, 5 degree rake angle. Your "force definition" that you paid for is for that specific material and tool combination. You can't apply that to a tool with 35 degrees of helix. The coefficients are different.

The place this product does really shine though is on long running jobs with lots of material removal.

I saw a demo of a part that roughed with the same tool for over 80 hours, on a setup that wasn't very well designed, so rigidity was a huge problem.

Vericut Force paid for itself on this job by cutting about 40% of the time off the roughing path, eliminating the chatter problems they were experiencing, and tripling the tool life.

So for the right application, it absolutely has its place. However, in a job shop environment, where tools/materials are constantly in flux, I would suspect that Opti-path is more economical.

Why won't you let Opti-path create new code? That is the true beauty of using it. When you do this, it does not change the trajectory of the path, at all. The overall path that the cutter takes is 100% the same after you create the new code. What it does is to break up the motion into smaller segments, and applies a different feed rate to each segment.

In order to get the best performance, I recommend you do this:

1. Start by defining a parametric tool in Vericut.
2. Run the NC Code through Vericut using Opti-Path, let it create a new NC Program for you.
3. Save the new NC Code file with a different name (my_program_opti_whatever).
4. Reload the job, and load the optimized NC Code file. Turn off Opti-Path.
5. Load the DXF/Solid tool, and run the "correct" tool geometry against your newly optimized code, to see where the "real" cutter is going to hit or clear.

By running Opti-Path with a generic "parametric" tool, it should make the process of creating the optimized program much quicker, and will let you get away with running the DXF tool definition, once the program has already been optimized...

[YoDoug®]

4 hours ago, gcode said:

VC Force.pdfI rebuilt the tool using a Sandvik solid model and Optipath chip thinning is running with a properly defined tool now.

My seat of Vericut has the Force setup page in the tool definition and it does look intriguing.

I haven't tried it though. I think it's an option that must be purchased and the Force page is just eyecandy to lurie

you into pulling out your check book

\

see attached screen shot

 

 

 

 

 

 

 

VC Force.pdf

Tom,

Have you ever looked into an adaptive spindle function for your machines. We add TMAC from Caron Engineering to a lot of machines we sell. This option can measure spindle HP down to .001 HP increments and adapt the feedrate to maintain target HP levels. It also helps you to make sure each tool is doing the same amount of work before it is expired. 

[gcode]

Colin,

by using a CAD model, (a Sandvik step file) to define the tool, Optipath ran correctly in chip thinning mode

It's slowing down in the corners and speeding up leaving the corners.

Right now the feed changes are abrupt, 78ipm to 50 in one block

I'd like it to do this gradually, but haven't figured that out yet

[Colin Gilchrist]

Would you be interested in some one-on-one training in Vericut/Opti-path?

[Matthew Hajicek - Singularity]

4 hours ago, gcode said:

Colin,

by using a CAD model, (a Sandvik step file) to define the tool, Optipath ran correctly in chip thinning mode

It's slowing down in the corners and speeding up leaving the corners.

Right now the feed changes are abrupt, 78ipm to 50 in one block

I'd like it to do this gradually, but haven't figured that out yet

For the Mastercam Highfeed Filter you can set the "Up feed rate scale factor" and "Down feedrate scale factor" to adjust that.

[Watcher]

Optipath is the best tool for what your after in this specific case. 

Let it create code and it will break your feeds to you. There's a setting that let you define the max . feed change so you have absolute control over the approach and departure in terms of feed rate transition... 

[Newbeeee™]

On ‎23‎/‎06‎/‎2017 at 7:26 PM, YoDoug® said:

This option can measure spindle HP down to .001 HP increments and adapt the feedrate to maintain target HP levels

THAT is impressive.

[BenK]

On 6/23/2017 at 1:26 PM, YoDoug® said:

Tom,

Have you ever looked into an adaptive spindle function for your machines. We add TMAC from Caron Engineering to a lot of machines we sell. This option can measure spindle HP down to .001 HP increments and adapt the feedrate to maintain target HP levels. It also helps you to make sure each tool is doing the same amount of work before it is expired. 

 

That is an impressive function. If I ever started a machine shop I would definitely give it a try.