Vericut question

[Bob W.]

Can Vericut be configured to warn if tool loads or engagement limits are exceeded? For example, if I am running a dynamic toolpath with a 20% stepover and at some point the tool becomes 100% engaged can it be configured to flag this? With all of the high speed toolpaths running now this has been my biggest issue with catching mistakes or glitches using verify or similar because the tool is almost always running in feed mode and verify is looking for collisions in rapid.

 

I snapped off a 1/2" mill today because of a glitch in the optirough toolpath sent the tool at 1/2" deep and 100% engagement with a very aggressive feed rate. The tool made it about 1/4" and it was right in the middle of the toolpath. Verify and Predator both missed this, which I would expect.

[Chris Rizzo]

glitch in the optirough toolpath

 

I've had some sketchy results lately as well. I've been so busy haven't had time to really investigate and send them in to qc if needed. Seems to be on entry moves.

[Bob W.]

Seems to be on entry moves.

 

Right, mine happened on the entry move between depth cuts. The entry was medial and I will try to avoid that strategy in the future.

[Tim Johnson]

Can Vericut be configured to warn if tool loads or engagement limits are exceeded? For example, if I am running a dynamic toolpath with a 20% stepover and at some point the tool becomes 100% engaged can it be configured to flag this? With all of the high speed toolpaths running now this has been my biggest issue with catching mistakes or glitches using verify or similar because the tool is almost always running in feed mode and verify is looking for collisions in rapid.

 

In your project Tree under the motion tab change your fast feed to the fastest number you want the tool to cut material. Any feed higher will set off an error note in your logger. That is a global parameter for each setup however. It would be nice to set the fast feed rate in the tooling section for each individual tool.

[cobra95kev]

Yes you can do exactly what you want and you don't even need an optipath license. Go to your tool list in Vericut and right click on the tool you are wanting to check and select add optipath I think is what it says. You then can set limits for that tool based on various criteria, including volume removal, stepover, and depth of cut. I will not run any dynamic or optirough toolpath without doing this. I find the volume removal to be the best indicator for the dynamic/optirough paths. I avoid medial entry whenever possible to avoid volume removal spikes I use helix entry. Also make sure your rounding radius is at least as big as your stepover to avoid possible spikes.

 

I almost forgot after you set the tool up for optipath limits in Vericut you then need to in your setup at the top of your tree check the box that says "Check Cutting Limits" for this to actually work. This is in Vericut version 7.1 whatever.

 

 

It would be nice for mastercam verify to be able to calculate volume removal in real time like this in Verify. Would be a good enhancement request!

[Jon @ NOWHERE]

Yes you can do exactly what you want and you don't even need an optipath license. Go to your tool list in Vericut and right click on the tool you are wanting to check and select add optipath I think is what it says. You then can set limits for that tool based on various criteria, including volume removal, stepover, and depth of cut. I will not run any dynamic or optirough toolpath without doing this. I find the volume removal to be the best indicator for the dynamic/optirough paths. I avoid medial entry whenever possible to avoid volume removal spikes I use helix entry. Also make sure your rounding radius is at least as big as your stepover to avoid possible spikes.

 

I almost forgot after you set the tool up for optipath limits in Vericut you then need to in your setup at the top of your tree check the box that says "Check Cutting Limits" for this to actually work. This is in Vericut version 7.1 whatever.

 

 

It would be nice for mastercam verify to be able to calculate volume removal in real time like this in Verify. Would be a good enhancement request!

 

 

So we don't need to have the optipath option to do this? It's great if that is the case!

[cobra95kev]

No, no license needed just to check limits. It will stop in the program and tell you it exceeded the removal limit you set, you just can't do anything with it as far as having optipath fix it. What I have done when it only exceeds in a few spots is to edit the NC file to slow the feed slightly in the areas where it gets overloaded.

[Jon @ NOWHERE]

Cool, I will give it a shot. Although we haven't went to 7.1 yet, so hopefully it works in 7.0.

[Chris Rizzo]

Bob, have you used the tool-overload feature at all on your Haas machine? You can set it to alarm, feed hold, or reduce feedrate. Although not sure if it would react fast enough.

[Bob W.]

Bob, have you used the tool-overload feature at all on your Haas machine? You can set it to alarm, feed hold, or reduce feedrate. Although not sure if it would react fast enough.

 

I have and most tools are set pretty low (~25%) depending on what it is. The 1/2" end mill is quite a bit higher though since I use it for most of the heavy cutting. That feature has saved my butt once before.

[neurosis]

Just a forewarning on helical entry using optirough. Ive had several occasions where helical entry is selected and it just shoots the cutter straight down in to the material.

[Bob W.]

Just a forewarning on helical entry using optirough. Ive had several occasions where helical entry is selected and it just shoots the cutter straight down in to the material.

 

Was this shown in backplot?

[neurosis]

Yes. It shows in backplot. You can see it in verify as well but it doesnt error because it feeds straight in to the part at a high feed rate rather than helical. I am working on a part right now that I can reproduce this error on. In fact, I havent been able to avoid the problem as of yet. I am using Volumill for the 3d roughing.

[Colin Gilchrist]

Neurosis,

 

Are you using Helical for your entry move? I've seen the plunge error when using Helix before. I've been able to get it to work (usually) by trying a smaller and smaller helix value. I usually try and stick with "Profile" entry, which is a helical style ramp. I'm having great success with using the "entry speeds and feeds" with a Dwell value to let the spindle speed ramp up.

[neurosis]

On this particular part it doesnt seem to matter what type of entry I choose. It just plunges straight in to the material. Ive tried all entry methods and changed the helical rad, etc. So far the only change that has worked was the change to Volumill.

 

The area that is an issue, the floor ramps down against a wall to make a closed angle. Its a slight closed angle but closed. Imagine a V shape only slight.

 

The rest of the part is open and pretty regular shaped. I am using Optirough with core selected.

[Zoober]

Cool, I will give it a shot. Although we haven't went to 7.1 yet, so hopefully it works in 7.0.

Just updated Vericut to 7.1.2 this morning. Ran a couple of tests with X4, X5, 7.03, and 7.12

The combo to get the X4 style tool holders into Vericut is Vericut 7.1 and X5 using the Vericut interface.

And IT IS SWEET.

I have some shrinker in shrinker holders in MCX, and they came in nice...