corner radius too small? - Hurco VM1

[Marshal]

We've got a Hurco VM1, and are trying to cut a few small holes (radius 0.1075" and 0.0675") with a 1/16" endmill. We run it through MCam, and it posts just fine with no errors, but when it pops up on the mill it says "corner radius too small". Now, we cut the same pattern earlier, with the same size holes, and didn't have this trouble (and yes, it's kicking out the error on the same line, regarding the 0.1075" hole).

 

Anyone have any experience dealing with this issue, or something similar?

[Marshal]

I should add that we're using a 2D contour toolpath for the entire thing, at a depth of -0.022"

 

As well as using MCam X4, MU3

[nhraguy]

Maybe check your cutter comp on the machine. Just guessing. We have had that problem on our fadals every now and then and I beleive it was related to the cutter comp.

[Marshal]

thanks for the tip. I'm no expert in machining (not by a long shot), so what do you recommend it be? Hopefully we'll be able to find that setting.

 

What doesn't make any sense is that it has no problem with the 0.0675 radius hole (0.0363 radius toolpath), but it kicks out the error at the 0.1075" hole/slot (0.076 radius toolpath). So it doesn't have an issue with a smaller radius, but puts out an error on a larger radius.

[veedubnut115]

chances are it is a cutter comp issue. I would try posted the code, with computer set as the comp. See if it works. If it does then it totally has to do with how Hurco is using cutter comp. I've had problems with our hurco and cutter comp before. Sometime wear works, and sometime control works. All depends on the part...Hurcos are really tempermental

[Marshal]

You aren't kidding. The thing has a mind of its own most days. I'll check it out tomorrow and see what happens

[Superman]

I agree with the comp issue, but more machine related than mastercam.

 

The problem is ore than likely on the arc lead in /out, 9/10 times it would be the lead in arc.

 

Try using a perpendiculr line only

or if you have to use an arc, try one that uses quadrants ie 90° or 180° sweep.( cuts back on the calculation/rounding errors)

 

You can add a point at the hole centre in the operation geometry and check on the "use entry & exit point", and set the line length to zero

 

The point centre should be above the chained contour for each chain

[Fred @ Slate Industries]

If you have the Hurco ISNC option, run your G code ".NC" in that "Editor" not Basic NC.

Use "Wear" in MC as your cutter comp setting.

To Use cutter comp at the mighty Hurco go into

Tools/ offsets/length/Radius Use the draw function to see your neg or positive numbers effects on the toolpath.

Length will give you an error and won't run,

Go to Radius !the pages look identical.

 

15 years of Hurcos here, not a single minute

in there Conversational editor!?!

[Marshal]

Ok, we've tried a couple of things, and some clarification is in order.

 

First, it does the small holes without a problem. It will also do a hole the size of the larger one (0.1075 radius), but will not do a slot shape that's two 0.1075 radius circles separated by 0.075" at the center. It also won't do a slot mill, which we just tried

[Marshal]

Well, we managed to fix it by breaking the arc at the center of it. It seems that the Hurco didn't like such a small 180 degree cut or something, and doing 90 degree arcs fixed the problem.

 

Stupid thing lol

[specprogrammer]

We get the same error often. I change to computer for compensation type. It has to do with the arc on radius (or off). When you check the draw screen you will see some funky arc that shouldn't be there. When I first started seeing that error I went through each line of code individually till I came up with the solution. Thats where it happens when the cutter comp turns on or off. Yes sometimes it will do a small arc and the next arc could be twice as big and it'll gag.

[Dave.L]

I don't know if this will help, I only skimmed the posts, set your comp in MC to wear that way the moves will be only .001 or so.

 

All we use hear is wear comp.

[Marshal]

Thanks for the tips. Breaking the arc seems to work fine, and it's just as easy for the work we usually do as changing the comp settings.

 

We usually just leave the comp setting at computer, and let it do it's thing. More than anything because I sure as heck don't understand the difference, and our old machinist isn't entirely sure either lol

[Dave.L]

quote:

---

We usually just leave the comp setting at computer, and let it do it's thing. More than anything because I sure as heck don't understand the difference, and our old machinist isn't entirely sure either lol

---

Comp set to computer means MC will offset the toolpath by the radius of the cutter you define but won't output cutter comp G41. So, you should only use this for features you will never need to adjust.

 

Comp set to control means MC will output the path as the part (no rad offset) and you need to specify the tool rad at the control. This option will give you G41 output and you will get errors all the time based on tool rad values.

 

Comp set to wear is the same as computer but you will get g41 output and you can them adjust your tool path at the machine by making very small offsets.

 

We only use wear here.

 

Does that help you understand?

[André Lapointe@In-House Soluti]

Computer compensation means that the tool radius is compensated in Mastercam based on the tool diameter define in your operation. If your tool diameter changes on the machine, you need to change it in MC because there is no compensation call made (no G41/G42 for example).

 

Control compensation means that the tool radius is compensated by the control on the machine. This means that in the control in the diameter (or radius) offset page (I don't know how it is done on a Hurco, some other may help you on this) you need to enter the exact value of the tool currently in the machine. So if the tool diameter change no need to change the program, you can change it on the machine. Now keep in mind that usually you need a linear lead in at least equal to or bigger than the tool radius in order to let the machine compensate properly. Also you will have problem if you try to do arcs that are smaller than the compensated value.

 

Wear compensation is a combination of both computer and control. Which means that MC will output the code already with the radius offset based on the tool in the operation but it will also output the compensation code call in the NC alowing you to adjust the tool radius on the machine based on tool wear. Usually rencent control have a separate page for wear offset that you enter only small value like Dave mentioned representing the tool wear. It not only allow you to compensate on the machine for small variation, but also will give much less problem with arc that have a radius close to the tool diameter, not to mention the lead-in length that only needs to be equal to or bigger than the maximum wear that you tolerate on a specific tool, instead of the radius of the tool.

 

I hope it may help you understand a bit more the differences between the different compensation mode.

[Superman]

Some machines, ( new or old ) don't like to do full arcs

 

You can set mastercam to automatically break circles into 180° or 90° arcs.

 

Doing this can also force greater accuracy into a machine that doesn't have tolerance control ( lag in the axis motors on higher feedrates or when the next block of code starts when the tool is in the "in-position" target area of the programmed position )

[Marshal]

I guess I understand the different comp controls, but the way this company is run, I don't think we need to worry about anything other than computer comp.

 

I think Superman's got it nailed, that our goofy xxxx mill just doesn't like to do full arcs. It'll do circles, and 90 degree arcs, but not 180's. Breaking the arcs fixed the problem, so I'm going to stick with doing that should the problem arise again

[Dave.L]

quote:

---

I guess I understand the different comp controls, but the way this company is run, I don't think we need to worry about anything other than computer comp

---

Are your tolerances +/- .1

 

I can't imagine making parts without cutter comp.

 

Trust me, start using wear and making adjustments, you will never go back.

[Marshal]

The last thing I want to do is confuse our machinist lol. I design most of the stuff, and help out programming a little bit. He learns things from me and I learn things from him, but he's not so good with changing the way he does things.

 

For everything we've done so far, leaving it at computer seems to work just fine. We don't do huge production runs, and the cutters get replaced when he thinks they're dull.

[Dave.L]

I can lead a horse to water but I can't make him drink

[K2csq7]

Marshal, do you ever use a re-sharpend end mills?

[Marshal]

Keith, I'm sure our machinist has used them, but I don't think they bother anymore. For the cost of the cutter, it's not cost-effective to get the majority of them sharpened. It's just easier for them to buy new cutters when they need them, which is pretty much the policy of this company. Their big policy is: "if you need it to do your job, we'll get it for you", which almost explains why I have a $3000 monitor for my computer, and a $4000 computer to run solidworks and mastercam. It also almost explains why they spent 30 grand on a rapid prototyper recently, just for me to use lol

[K2csq7]

To each his own!!!

[Dave.L]

quote:

---

It also almost explains why they spent 30 grand on a rapid prototyper recently, just for me to use

---

OK Marshall, but nothing will explain the lack of using cutter comp

 

It's not Rocket science, you and your machinist can handle it for sure.

[MotorCityMinion]

Gotta agree with Dave here. I set my Op defaults at WEAR, use IJK's, and break at 180. just because.