EasyStone question #47

[ChrisYaughn]

I know there is a way to auto filet inside corners so that breakers don't take off too much material or jam into an inside radius.

Is there an elegant way to slow down profile wheels as they go into inside corners? On most parts I run a min inside radius of 3 or 3.5'' so it is not a big deal. But on sinks, I am cutting it close on the radius a lot, barely getting it bigger than the wheel and have to baby sit it thru the corner. Backing the feed rate way down while it is in the corner.

Any thoughts?

[coolhandchris]

I know there is a way to auto filet inside corners so that breakers don't take off too much material or jam into an inside radius.

Is there an elegant way to slow down profile wheels as they go into inside corners? On most parts I run a min inside radius of 3 or 3.5'' so it is not a big deal. But on sinks, I am cutting it close on the radius a lot, barely getting it bigger than the wheel and have to baby sit it thru the corner. Backing the feed rate way down while it is in the corner.

Any thoughts?

You need to split the line going in to the corner in draw. Then when you select the lines to be machined, add kit, then click on the lines that you want to vary the feed on. 'feed variations'- set to desired speeds. I might be a little off in the steps, but my computer isn't running so this is just from memory.

In the kit there is an option for auto fillet, fillet *1st tool special or no fillet. Select *1st tool special to make it auto fillet to the size of the breaker (1st tool).

Call me tomorrow, I will walk you through both of them.

[ChrisYaughn]

just tried it.

I followed the explanation and it looked liked it worked. Just clikc on the slow areas then right click and modify thier feed rates. I'll try it on the machine tomorrow and see if it works.



Thanks

Riding the knob on sinks is a pita.

[coolhandchris]

I have my sink set as fillet internal corners. It will error out if you try and generate code and the radius is too small for the tool. At least I think it will.

[scott m]

That is one thing I hate about easystone. Yes, it will error out and you will get "internal radius too small" so you have to make your drawing fit the tool.....Alphacam will just to the best job it can. So even with a 90 degree corner it will work, with certain tooling combination exceptions.

I assume Chris, you have a "sink" kit and a Z kit. If this is the case, you set it up as chris is saying and you will be good to go.

There is no substitution for just turning the work knob down a notch though......

[Ken Lago]

That is one thing I hate about easystone. Yes, it will error out and you will get "internal radius too small" so you have to make your drawing fit the tool.....Alphacam will just to the best job it can. So even with a 90 degree corner it will work, with certain tooling combination exceptions.

I assume Chris, you have a "sink" kit and a Z kit. If this is the case, you set it up as chris is saying and you will be good to go.

There is no substitution for just turning the work knob down a notch though......

Alpha cam will do it with the fingerbit but not the other tools.

[Nick]

That is one thing I hate about easystone. Yes, it will error out and you will get "internal radius too small" so you have to make your drawing fit the tool.....Alphacam will just to the best job it can. So even with a 90 degree corner it will work, with certain tooling combination exceptions. ......

That is not true. You can do a rectangle with 90* corners and apply any tool you have to it and it will do the absolute closest it can to 90*(smallest possible radius).

[scott m]

Ken, my alphacam is set to do it with any profile. Nick, the version of Easystone I used would error. I verified this with Cevin at coverings.

[ChrisYaughn]

Nick,

Mine errors out with profile wheels but will do it w/ the fingerbit.

[Nick]

?????

[ChrisYaughn]

I can cut a 90 degree inside corner with the finger bit and you just get the radius the size of the bit. But if I try to run profile wheels thru a 90 degree corner I get an internal radius to small error.

So it has to be a setting somewhere , right?

[scott m]

I think it is what chris v is talking about with the auto filet. I think you have to set the kit up like that. I don't run easystone for the breton so I can't tell you or even look at kits to figure it out.

[ChrisYaughn]

Got it. But even auto fillet is going to load the crap out of the tool when it hits the corner and is in contact on %25 of the face of the tool.

I am digging the rick click, adjust feed speed trick.

[Jqualey4130]

The settings for what Radii your tools will do or not are in Database in the Draw section. If your mill bit is 1 inch in Diameter, it should be able to mill a 1/2 inch radius. There is a value somewhere in the software that gives the machine a little extra room to not bind the bit. If it won't do 1/2 inch it will do 9/16th's. Also, if your database setting is greater than the setting of the tool in the offset menu on your controller, you will get an CRC alarm on your macine. If you change out your mill bit and don't update the database setting this can happen. Or if there is a small little radius in a sink DXF that you didn't clean up well enough this also can happen.

Chris, Another trick w/ the auto slow is to break your line an inch or so before the radius and give it a speed step down before the actual corner. If my Y breaker is going 80 IPM and I want to feed it thru a 2.75 in internal radius, I would use the broken line before the corner to drop to 40 before it hit the corner. And in the corner I might feed it at 25 ipm. The reason I do this is because the tool is measured from the center of the spindle and if your breaker is 100mm wide, It is already in that corner before the speed gets dropped down. Blade breakers don't suffer from this for some reason.

Justin Qualey
Qualey granite and Quartz

[DavidL]

In my software if I draw my corner as to lines intersecting rather than a radius I can run any tool into there without an error. If I have a radius, then yes I get an error. Is that the same for EasyStone?

[scott m]

Ok, that all makes sense. It is compensating for the diameter of the tool in the cam, not on the machine entirely. What Alphacam does is follows the edge to be routered and on the machine it adds the radius of the tool. The problem with AC is if you follow a small tool with a large one such as my z set 80mm with 120mm polishers, you will blow up the polishers.

[ChrisYaughn]

Chris, Another trick w/ the auto slow is to break your line an inch or so before the radius and give it a speed step down before the actual corner. If my Y breaker is going 80 IPM and I want to feed it thru a 2.75 in internal radius, I would use the broken line before the corner to drop to 40 before it hit the corner. And in the corner I might feed it at 25 ipm. The reason I do this is because the tool is measured from the center of the spindle and if your breaker is 100mm wide, It is already in that corner before the speed gets dropped down. Blade breakers don't suffer from this for some reason.

Justin Qualey
Qualey granite and Quartz

yep.

[Jerry Kidd]

For Chris and Chris – Chris V. your special 1st for the breaker/pre-cutting bit is something most people will not have. This is a development that just arrived in the software during the last year. The application arrived because there was not really a place in the software for the use of the pr-cutting bit. There were possible ways to get the tool in with the profile kit and there was a way to run it as a milling tool. Saving you a long explanation neither fully addressed elegantly using the tools. Now you can add the tool to the profile kit and get the full safety features of the true tool diameter. With this application you get the option of special 1st for the fillet internal corner option in the kit. Now the use of these tools is elegant and safe.
So the easy solution of what Chris Y. needs is in an internal corner use both ideas. For the breaker/pre-cutting bit that he is using as a milling application use fillet internal corner option and this will leave a lot more material in that corner for the 1st tool of the profile. So now use the Feed Var option just before entering that corner with the profile set and let it have the opportunity to remove all that material gently. The combination provides a smooth elegant solution to this challenge.
During the last year and a half Easy Stone has been very open to modifying the software to make the whole Cad Cam experience much easier. I have not kept count but I myself have made suggestions to well over 20 modifications that they have embraced. Be it for counter tops or 5 axes work a lot has changed during that time. I am very impressed with their desire to become the complete software package. There is a lot more coming up in the future that is very exciting. The largest stone company in America is quite happy with Easy Stone and what it is doing for them. I feel really sorry for you guys with older copies…

Jerry Kidd

[StevePaul]

The internal radius check that takes place in the software is a mirror of the tool radius check on the control. The software is merely trying to filter the error before it gets to the machine... which saves you time.

Simply put: The internal radius to be machined must be equal to or greater than the radius of the tool plus it's over-material value.

In order for the software filter to be accurate, the tool radius in the software must equal the value at the CNC machine.

The software and CNC control will allow you to jam any tool into a non-radiused or non-filleted corner.

There is a time and place for every method on a CNC and sometimes this is the best solution. It is typically used with similar sized tools, mostly with smaller radii and always at your own risk.

.

[ChrisYaughn]

The software and CNC control will allow you to jam any tool into a non-radiused or non-filleted corner.

There is a time and place for every method on a CNC and sometimes this is the best solution. It is typically used with similar sized tools, mostly with smaller radii and always at your own risk.

.

Indeed It Will

[Nick]

The internal radius check that takes place in the software is a mirror of the tool radius check on the control. The software is merely trying to filter the error before it gets to the machine... which saves you time. .

Not entirely true on an OMAG that calibrates wheels via the renishaw probe. In theory, the machine regestered diameters will just keep getting smaller as the tool wears, but your initial caliper measurement for software and first series of probes will be differnt plus or minus. So if right away you went the bare minium, you could pass on software and get warning and stop at the machine. That said, lying to the machine about breaker bit radius causes programs that the software likes and the machine does not, that is more common.

[Jerry Kidd]

Nick, I am confused as to your comment - are you talking about the same application in an un-filleted corner like Steve is? I am a little lost in what you are saying and Steve just accurately described that situation more eloquently than I have ever heard it said. In fact I intend to do my best to say in the same way to all of my future trainees.

Jerry Kidd

[Nick]

I may have misunderstood. I was thinking that my machine has different min. radius numbers than my software due to the fact that the tools are probed and constantly changing. This should alwyas be by hairs and always smaller than the software so no issues, but I have once with a new tool and quite a few times with a breaker bit(because I intentionally have differnt numbers in the machine, written a program that the software says OK to and writes the code, and the machine, with it's measurements in the tool file gets to that bit and stops about 2-5 ft. before that inside raduis when on that tool in the cycle when it realizes it is .002 too small of a radius, and gives me a "bloc indicate......"

Am I thinking about something way different? I know Steve is mega smart and I just thought what I am reffering to as an OMAG/probe thing that he wouldn't have experiance with.

No, not in an un filletted corner, but in a radius I made, like say 2.3 works in the software for my ogee set new, but failed at the machione. I now do 2.35 automatically, no issues anywhere. Although as worn as my ogee set is NOW I bet 2.3 will work at the machine when it did not when new because of recent probes lowering the intial first ones that were a hair larger than what I calipered and entered in the software. I am not explaining this well am I??? I could be talking about something different???

[StevePaul]

Thanks Jerry.

Nick,

The software should always get the maximum radius plus the overmaterial value. If the initial probe cycle is larger, increase the software value as well.

Establishing a max value in the software and a safe minimum radius, like you are doing...is the best way to keep internal radius errors from stopping the machine.

The value at the machine should get smaller with each probe cycle, which would steadily increase the margin between the initial and current measurements, in your favor, at the CNC control.

If your probe has a calibration cycle, run it often to maintain accuracy. The reference position for the probe can change if any of the axis are serviced, adjusted or worn. (Esp if the tools consistently measure larger after a probe cycle..)

We recommend working accurately with tool measurements whenever possible... fudging will eventually cause trouble and cost you in one way or another.

BTW: most CNC controls look ahead up to 15 lines and will flag something it can't resolve before arriving at the geometry. Jumping to "block by block" or line by line mode will usually override the look-ahead if you want to identify the line with the problem.

[coolhandchris]

If your probe has a calibration cycle, run it often to maintain accuracy. .

I run mine everytime I turn on the machine, otherwise it will ask me if I want to run it every time a tool set to probe comes up.