cutter's compensation

[Brendan P]

Also,machine controls dont like to turn c.c. on or off on an arc.

Usually you will get an alarm

[Thad]

quote:

---

Usually you will get an alarm

---

Not on a Fadal.

 

Thad

[JazzBass]

quote:

---

Don't forget that you CAN'T use WEAR comp if you choose to use the Highfeed option - it will do wierd things to you (you need to use computer comp).

---

+1000 Gary,

 

I hear it will not be fixed in X.

[35K chipper]

I program the part to the nominal print demension and use the cutter comp in the machine to adjust for tool size differences, wear, plating buildup or electro polish reduction. The mc geometery will match the print and the part can accomodate all the outside variables the customer might require.

[Dave anderson]

This is a good post as i have a small 3 axis knee mill anilam and i notice when doing inside and outside circles they are usually off .005" to .010 with the outsides being closer to tolerance than the insides I use cutter comp computer . im not sure why my inside circles are slight off more than my outside circles though?Ps im new to this so bear with my ignorance pls i have tried new endmills and have had same problem and i know work is held steady i wonder if possibly the gibs may need adjusting though machine is in good shape but ive never adjusted the gibs . so if i use wear when programming my tool offsets do i put in a value for the X as opposed to the way my control works i just touch tool to top of part and enter z and x display position? in the past i have just changed values in xy stock to leave in mcam the alleviate this problem but that isnt teaching me anything. thanks guys.

[TheePres]

Wishing that Mastercam would add cutter comp options on "surface finish contour".

[robk]

quote:

---

when doing inside and outside circles they are usually off .005" to .010 with the outsides being closer to tolerance than the insides I use cutter comp computer

---

Try slowing down the feedrate and see if they're closer to size. Might be that your machine is not keeping up around the corners.

[P_Scott]

Dave anderson,

 

robk brought up an excellent point. It could be the feed is too fast for the machine to keep an accurate circle. Cutter compensation is a way to eliminate the "leaving stock" in Mcam. Whether you use Control comp or Wear comp, you would still have the option to change the size of the cutter at the machine. This wouldn't require that you go back into Mcam and leave stock or remove stock that was previously left on. With Computer comp, Mcam is the only place you could change the size of the tool, or do as you've done in the past. This takes time that many programmers or operators don't have. HTH

 

35K CHIPPER,

 

Welcome to the forum. Control comp is OK for many applications. Do you ever encounter a "tight" situation where you don't have enough room to turn CC on with the amount of Entry (>50% tool dia.) you're required to use with Control comp? I've had clients ask me why they have a "gouge" at the beginning of a contour operation when they're using Control comp. This is a result of Control comp being activated by the time it reaches the end of the first G1 move. With Wear comp, the compensation is applied at the beginning of the first G1 move. This tends to eliminate any "gouging". HTH

[heeler]

OOPS

[heeler]

Peter Scott,

 

I to like to use control/Full cutter comp.

 

" Do you ever encounter a "tight" situation where you don't have enough room to turn CC on with the amount of Entry (>50% tool dia.) you're required to use with Control comp? "

 

This used to be a problem, but now there is the plunge after first move option on the lead in lead out page. No more problem.

 

Many times I have been running the machine and could see there was a problem from the code. Holes not where they should be, end of part to long/short.

 

We do argue here alot about which is better. Seems to me that most of our programmer prefer wear because they don't really understand how to apply/unapply cutter comp. Many times I find errors even using wear, because they don't get it applied in x and y before doing an arc move.

 

 

HTH

Glenn

[P_Scott]

heeler,

 

I'm not suggesting that Wear compensation is the only one to use. Before the "plunge after 1st move" switch was introduced in V9.1, the "gouge" effect was a real issue. I'm glad you use that feature and have experienced no problems since. I prefer to use Wear comp because that's what I learned, in the shop, setting up the machines and running my own programs. There are benefits to knowing all types of compensation and what they will allow the programmers and operators to accomplish.

[g huns]

quote:

---

Wishing that Mastercam would add cutter comp options on "surface finish contour".

---

+1 to that

[drago]

Question: where on the control do I make the change of .010" wider? Under Offset -- Tool radious -- wear??

 

 

Since you have "tool radius" column available you don't have to mess around with different offset numbers (D41 for tool 1) like somebody already mentioned it.

 

Just input the amount you want in "tool radius" column when the tool is fresh. Wear column is for compensation at a later point in time, aditional to "tool rad", and on some machines you can only change wear comp value incrementaly - If there was a value of .007 in there and you type -.003 it's gonna subtract it and you'll have .004

 

Basically, wear comp is a comp for your tool rad comp.

 

hope this helped.

[apprentice]

Thank you, guys. All your help is truly appreciated!!

[Dave anderson]

I will try cutting some circles this weekend and see if the slower feed rate helps. Im also gonna have a look at the jibs to see if a small adjustment would help. I know my machine is nothing like the machines most of you use but for the little stuff i do its ok but a little more accuracy would be nice.

[Guest CNC Apps Guy 1]

If you have Tool Comp C, you'll have wear values in the offset table, if you don't have Tool Comp C, you'll have to have different H's and D's.