Cutter Compensation

[AdamB13]

I currently run version 9.5 and I am thinking of upgrading to version 10.
My question is, does version 10 support cutter compensation?
Any input is greatly appreciated.

[mtylerfl]

Here is a thread discussion that addresses “cutter compensation”:

http://forum.vectric.com/viewtopic.php? ... on#p239518

[AdamB13]

Thanks, mtylerfl but I need actual cutter compensation using G41/G42.
We run several programs for a customer at night when we are not cutting cabinets. I can't sit around and wait for the CNC operator to change bits and then re-calculate the toolpath. I need it to do it on the fly since they might change a bit during their shift.
When I went to the Vectric user group last year in Chicago I asked about it and they said that it was in the works.
Before I can get the owner to spend the money to upgrade he wants to make sure it will handle that. If not then we will have to wait until it can. Version 9.5 does everything we need, minus the cutter comp.
If anyone knows how to modify the post to add the G41/G42 I would be willing to go that route.

[Leo]

I have been asking for G41/G42/G40 for a long time.

It is not a popular request.

V10 does not have it.

[AdamB13]

Thanks Leo.
That's what I was afraid of.
I'm really surprised that more people aren't asking for it. It makes life a lot simpler.
Maybe some wiz with experience modifying posts knows a way to have it add the G41/G42 into the code.
I have a copy of my post for Cabinet Vision which uses cutter comp but I am just not sure how to modify the V-Carve post to make it work.

[TReischl]

At first blush cutter comp seems like a fairly easy thing to do. . . then reality sets in.

Figuring out which way you are going around something is no big deal, and since the user tells the computer whether the cut is inside or outside that info is available.

Here comes the rub. . . .

A lot of machines read the cutter comp command, then it is implemented when the machine starts to move. In other words the cutter comp happens as the first move takes place resulting in tapers, etc. It is especially apparent for those who input large amounts of cutter comp. Some machines do not operate in that manner, so right away there is a problem. Then there is the whole thing of assigning comp registers to certain tools and people not paying attention to what they are doing. I know this because I have been there, done that in my former life.

Can it be done? Of course it can. The question for the developers is whether it is a useful feature for their user base. I always keep in mind that Vectric products are primarily targeted at carving, not precision machining where cutter comp can really shine.

I would like to have it too, quite often I am doing fairly precision work and it would downright handy instead of having to go and either change the hole size or cutter size. But I get it, these products are not targeted at machine shops.

Sometimes it helps to understand why something isn't done that we think is the best thing since sliced bread.

By the way, I got off easy when I had to do it. I was writing CAM software for lasers. My solution was to make all interior cuts counter clockwise and the exterior the opposite. Did that automatically and had an option to allow the user to override. On those particular machines cutter comp needed about .25 inch of motion to adjust. So I triggered cutter comp and then did a dummy move dance to get it going. No one ever convinced me that a laser cutting steel produced a better cut by "climb" or "conventional" milling directions. Laser beams don't spin. Oh, all cuts were on line in the software with the cutter comp being half the beam diameter.

[Leo]

I have written tons of code with cutter comp G41/G42/G40. Knowing how the code works is not so much the issue.

1) Is the machine control software capable?
Do they have the offset registers?
Do they support cutter comp?
2) Do people know how to use it? OK they can learn.
Then we need to talk about what to put in the offset register - cutter diameter or cutter centerline?
Right now - Vectric takes care of that and makes it easy.
3) Like MasterCAM or others it is not in Vectric software.
On - Right - Left would output the code
OR a switch to turn it on or off is not there.

I have no idea at all how to write the software behind the scenes in CAM.
I know it can be done, because other CAM software has it.

For me - I would like to have it, but, it's just not a show stopper for my stuff - so - I am just as happy.

[AdamB13]

Thanks TReischl & Leo.
I understand what you are saying about the customer base and the type of machines they are running.
I was just hopeful that we could have it in V-Carve as we are cutting about 1000 shelves per week and they need to be consistent.
For the shelves, I used Cabinet Vision to create the parts and output them to the machine. The only problem is that I don't have all of the control features of V-Carve to assign what parts are cut first and order of operations.
Because I can't control the cut order I do have a couple of pieces that move and are no good.
We are cutting 4' x 8' sheets and some of the programs take over an hour. I was able to take one program that I had done in Cabinet Vision and once we had V-Carve I was able to cut the machine time down by over 1/2 an hour because of the control I have.
These are not your typical shelves though. They have dado's for parts to fit into and holes to be cut for hinges. Without the cutter comp, the dado's width varies and so does the hole diameter so either the cleat won't fit or the hinge won't fit.
I will just have to deal with losing parts from time to time.

[TReischl]

Sheesh.

One of the problems a lot of us have is not building an assembly tolerance into our designs. A hinge is a good example. The manufacturer says they are 1 inch wide. So what do we do? We draw a pocket up that is 1.000 wide. That is nice, but depending on which die a hinge runs through it might be .995 - 1.005 or worse. I am just tossing some numbers in there for the conversation. The problem is apparent immediately, some hinges will fit, others won't. But one thing is for certain, a lot more will fit if the pocket is drawn to something greater than 1.005. Of course, the undersize hinges will have tiny gaps. Most people would never notice them, but being wood workers, we see everything, all must be perfect!

I recently did a walnut box that had small hinges on it. I measured them and then because I have been bitten more than once by this situation I drew them .005 oversize. That worked nicely.

Another thing that I have done is test cut a bit to see what it really cuts. A good way to get a really accurate measure is to clamp the material down and then make a cut all the way through (make sure you have both halves clamped securely). Measure them with a digital caliper BEFORE you cut, and then again after, the difference is how wide a cut the bit is really taking. Trying to put the little pointy ends in a 6mm slot is not the most accurate way to measure because that sharp edge collapses wood fibers depending on how much pressure you put on them. I don't do that much anymore because it is a bit fiddly and I am retired. So if someone doesn't like how I fit things together, oh well! BTW, this technique works great for saw blades so you know what they are cutting. Measuring the cutter is about the worst thing a person can do. Doing so does not take into account collet runout, spindle runout, machine flex, backlash, etc. After all, what it really cuts is the important thing.

Hopefully something in all that yapping will help you out a bit.

[tomgardiner]

I suppose duplicate V carve files with multiple cutter diameters would be a potential disaster.

[ger21]

I have a copy of my post for Cabinet Vision which uses cutter comp but I am just not sure how to modify the V-Carve post to make it work.

I believe that you could write a post that adds comp fairly easily, but you'll quickly find that you need to be very careful.
1) Be aware that comp will be added to ALL of the toolpaths, which you most likely do NOT want.
2) For comp to work, you'll need to always add lead in and lead out moves, and have the post insert the G41/G42 in the correct places. And you'll always need to cut ON the line.
3) Since V Carve knows nothing about your comp post, your post will always insert G41, or G42 comp, but not both.
4) This leads you into needing separate posts for G41 and G42, and you need to know when to use each one.

As you see, it's really not worth the trouble, and potential aggravation.

Comp is a wonderful thing, and most people do not understand how useful it is. Virtually all industrial routers use it for everything. It's indispensable in a high volume setting.

I use comp for all profile toolpaths on my Mach3 machine.