POST/RADIUS PROBLEM

[G Caputo]

Hi all,

 

I am milling a slot using a simple 2d contour and having a problem when it gets to a corner. It a a slot that is open (runs out of the part) on one end and has .750" radius in the corners at the other end. I am using cutter compensation in the control which the operator requested. I have created geometry above the solid and chained it. the geometry I created is an exact duplicate of the perimeter, 3.500" wide x 86" long with .750" fillets in the corners. I have also told the xy stock to leave to be .010" so I can finish this with an end mill at the final depth. I also do not have the filter on for the post to read "create arcs in xy".

 

The problem I am having is not necessarily the post or maybe a checkbox of some sort I am not seeing. I am using a 1-1/2" cutter and the program is creating arcs at the corners using circle centers, so when it gets to the corner it is trying to mill a .74" internal radius with a .75" radius cutter, which obviously can't happen. I am able to correct this by:

 

1) not filleting my chain at all so it sees a square corner.

 

2) putting a .76" fillet in the corner so when it cuts to +.010" it is then a .750" radius.

 

3) offsetting the whole contour by .010" and telling the xy stock to leave at 0.

 

My question is am I missing something obvious that would allow me to keep my geometry as drawn? Is it something that the post should notice and needs to be modified? Or am I doing this the correct way?

 

Thanks,

Greg

[Rekd™]

The problems is that you're using a tool with the same radius as the slot. You can't leave stock doing it like that. Either use a smaller tool, or make a bigger slot.

 

'Rekd teh If it sticks, jam it, if it breaks...

[Marty A]

hi gcaputo

 

i would run one program with no comp, and .010 in xy stock to leave. then one program with tool comp. hope this helps.

 

 

marty

[Fig sign]

The optimize must be checked in !

[Nominal]

The problem seems to be the inconsistancy of what you're trying to do. You want to leave .010 for a finish pass on the straight moves only, but still cut the corners to their finished size. I'd say you might aswell remove the corner radii in your geometry. This is not my favorite option, as I like to generate at least some contouring of the corners. But since your tool is the radius you need you don't have much choice. Filleting the corners on your geometry is kinda meaningless anyway since your not going to generate a circular move in your nc file. The best thing to do would be use a tool smaller in dia than the corner you need. If thats not possible the next best thing would be to use some of your tolerance and make the fillet larger than basic by whatever amount you can stand. I'm guessing by the description of your cut that you've got more than +-.001 for those corners. But if you choose to take the fillets out completely and just let the tool bang around in the corners you're probably going to get some deflection and thus some digging in. Comes down to what is less ugly for you.

[McRae]

Use an 1.25" cutter and your problem will go away!

[CAM-mando]

quote:

---

when it gets to the corner it is trying to mill a .74" internal radius with a .75" radius cutter, which obviously can't happen.

---

This wouldnt happen if you used WEAR or IN COMPUTER Comp !

 

As I have said before, you will create comp errors using comp in control. My suggestion is to tell the machinist / operator how things are going to be done now.

 

Personally I would also use a slightly smaller tool for the afore mentioned reasons, but this is an example of why it pays to let MC to what it does best and only use comp for wear / regrind (IMHO of course).

[G Caputo]

The problem I have is with using an 1-1/4" cutter is they are 2 fluted. Both tools mentioned are apft/apkt cutters from Carboloy. The 1-1/2" is a 3 flute. The part has 8 sides to it and each slot is anywhere from 60 - 86" long with each pocket around 3-1/4" deep. That's roughly 10,000 inches the machine will travel at approximately 3/8 depth of cut per pass. I put a 2 fluter in there and slow the feed down, I am gonna get my butt spanked.

 

I sorta lied to make the thinking easier... They are using cutter comp, stepping down the depth 3/8" at a time to +.002" per surface not +.010" on the side so they only have to take 1 pass with an endmill at depth taking off the .002" I just mentioned. I went with .010" before beacause the math in my head was simpler.

 

I was just looking for a way around mastercam's thinking that could get me into the least amount of trouble with them using cutter compensation. Or if they do use a tool with a 1-7/16" diameter, I don't want them to come back and blame me for how I toolpathed it and it didn't leave stock in the corners by going with just a rectangular toolpath drawn.

 

I don't yet have the mastercam's way of thinking in my head, been programming on the floor for 14 years and I can see how the hackers could screw things up. Sometimes I swear they even try to on purpose. Just trying to come up with the most logical and safest way to foolproof myself.

 

Thanks for the reply's and ideas. I think I am going to make the radius just a bit bigger to cover myself in all aspects.

 

Greg

[McRae]

quote:

---

10,000 inches the machine will travel at approximately 3/8 depth of cut per pass. I put a 2 fluter in there and slow the feed down,

---

Put the two flute cutter in, leave the feedrate alone. The thicker chip will be better anyway and the tool will handle it. If there was any problem, I would watch the overlap more than the feedrate...

[Rekd™]

quote:

---

Put the two flute cutter in, leave the feedrate alone. The thicker chip will be better anyway and the tool will handle it. If there was any problem, I would watch the overlap more than the feedrate...

---

+1

[Fig sign]

When you select tool compensation with aa control and have inner radiuses in the geometry less then a tool radius optimize is a must!

It eliminates arcs in the pass less or equal to the tool radius and helps to prevent gouging!

I do this kind of stuff all the way .

The beauty of this is that there is no need to edit geometry or fool the system with radius -0.01.

You make job one time and after that can copy

and use it with any tool you like!

If the next tool radius is less then the inner corner radius after regeneration you will get the proper arc in the toolpath !

 

Iskander teh :I am far more bigger than corner radius ,but properly compensated and optimized !

[G Caputo]

quote:

---

When you select tool compensation with aa control and have inner radiuses in the geometry less then a tool radius optimize is a must!

It eliminates arcs in the pass less or equal to the tool radius and helps to prevent gouging!

---

plasttav,

 

This is exactly what I was hoping to find, it works just as you said, with no room for error should it be used with a different tool, radius, etc. Thank you.

 

quote:

---

The problem seems to be the inconsistancy of what you're trying to do. You want to leave .010 for a finish pass on the straight moves only, but still cut the corners to their finished size.

---

Yet again I was trying to be stupid but safe and mastercam pulls through once again.

 

quote:

---

This wouldnt happen if you used WEAR or IN COMPUTER Comp !

---

This will never be an option for me 3 shifts, 6 machines with about 3000 handwritten programs up to 3000 lines apiece and all journeyman machinists running them. That would be great if it was just me programming them, but it's not and probably won't ever be.

 

Thanks to all who have responded, it just gives me more ideas to think about all the time, and all the different ways people do things.

 

Greg

[Fig sign]

Greg!

You are welcome!

 

Iskander teh :It is a night now and when I sleep I snore !

[Dan_AKA_ROY]

Tool radius optimization? Great tip! I'm glad I read this post. Learn something new every day! Thanks, Ghengis Khan! {just kidding, cool Avatar!)