CAMSLOT

[Lathe-Mill]

Good morning peeps, i am making a program for a camslot (slot along the dia. on the rotary head).

it's going from point A to point B on a giving angle, when I post it, it comes out a bunch of X's and A's moves, it does work ok in the machine,but, operators are crying that the don't like it cause it's too many lines and they don't know wich move is doing, so it kind of looks like a bunch of little lines making a radius, so far you understand what i am saying?...

 

How do i get the program to read like:

X.5 A0. (point A)

X1.0 A270. F5.0 (point

 

not like this:

N114 G42 D1 X.2076 A160.059

N116 A160.095

N118 X.2077 A160.13

N120 X.2078 A160.164

N122 X.2079 A160.199

N124 X.208 A160.233

N126 X.2082 A160.268

N128 X.2083 A160.302

N130 X.2085 A160.336

N132 X.2087 A160.37

N134 X.209 A160.405

N136 X.2092 A160.439

N138 X.2095 A160.472

N140 X.2097 A160.505

N142 X.21 A160.538

 

Thanx peeps

[Fig sign]

cARLOS !

Do you use filtering ?!?

[Lathe-Mill]

no plasttav, i dont think i ever use it

[chris m]

The easy answer to this is to tell the operator "That's the way the computer writes the program, push the f$#&ing button"

 

otherwise, make sure the post rotary setting is on "full rotary"

 

If that ain't it, probably filters.

 

C

 

[ 10-28-2003, 07:35 AM: Message edited by: chris m ]

[Lathe-Mill]

I never use the filters, dont know what they use for...sorry

[Lathe-Mill]

where do i set that full rotary chris?

[Lathe-Mill]

quote:

---

The easy answer to this is to tell the operator "That's the way the computer writes the program, push the f$#&ing button"

---

done that, they cry to the boss and boss said,can you just try to make it easy for them?

they cry babys here.

 

[ 11-06-2003, 03:10 PM: Message edited by: Lathe-Mill ]

[MACHINEMASTERG]

quote:

---

How do i get the program to read like:

X.5 A0. (point A)

X1.0 A270. F5.0 (point

 

---

on simple rotary jobs like that i just type it out in the editor just like you did here ...keep it simple dummie is what we were told

[Lathe-Mill]

quote:

---

...keep it simple dummie is what we were told

---

that is what i have been doing, but i just want the post to do it, avoid human error.

once the post is debugged, it will be ok. i think.

 

[ 11-06-2003, 03:12 PM: Message edited by: Lathe-Mill ]

[Fig sign]

A quote from help

quote:

---

When you filter a toolpath, Mastercam replaces toolpath moves that lie, within a specified tolerance, in a straight line with a single tool move. You can also optionally replace multiple linear tool moves with an arc move of a specified minimum and maximum radius.

 

How to filter toolpaths

The recommended way to filter toolpaths is to check the Filter check box on the Toolpath Parameters dialog box tab so that the toolpath is filtered as part of its operation. In the Mill illustration below, note the circled Filter check box. This same check box is also located in Lathe Toolpath Parameter dialog boxes.

 

When you filter toolpaths this way within the toolpath definition, the filtering is done automatically and the toolpath maintains associativity. When changes are made to the geometry, the toolpath can be easily regenerated.

Mastercam also provides two additional methods of filtering toolpaths:

 

¨ Right-click in Operations Manager and choose Options, Filter to filter only selected operations in the current MC9 file.

 

¨ Choose NC utils, Filter to filter any existing NCI file.

 

In this method, filtering is performed on the ASCII NCI file, which is created when the operation is post processed. Once posted, the operation is no longer associated to the geometry so the filtering has no effect on either operations listed in Operations Manager or on the toolpath operation itself.

 

Optimal toolpath filtering

Filtering toolpaths usually speeds machining by optimizing toolpaths, but it may increase processing time slightly. Achieving optimal results requires balancing several aspects of the part:

 

¨ Filter tolerance

 

¨ Cut tolerance

 

¨ Desired final machining tolerance

 

¨ Surface topology

 

¨ Advantages of arc moves versus linear moves in a particular part

 

¨ Number of points Mastercam looks ahead when filtering the toolpath

 

¨ Individual machine tool requirements

 

Unfortunately, no specific formula can be given to balance these aspects. While we provide some guidelines, experience and experimentation will provide the best direction.

Filter tolerance, multiaxis cut tolerance, and final machining tolerance

 

When working with multiaxis toolpaths, both the filter tolerance and the multiaxis cut tolerance contribute to final (net) machining tolerance. The filter is applied to the toolpath at the cut tolerance. We recommend that you set the filter tolerance to a minimum of twice the multiaxis cut tolerance. For example, if you want a net machining tolerance of .001 inch, then set the filter tolerance to .0007 and the multiaxis cut tolerance to .0003. For example:

 

This will result in a smoother, smaller toolpath at .001 resolution. Matching the cut tolerance to the filter tolerance (for example, .0005 each) is not recommended because the resulting toolpath will be too similar to the unfiltered toolpath to be considered optimized.

The same rules for tolerances apply whether you are using Filter from the right-click menu of the Operation Manager or from the NC Utilities menu.

Replacing linear moves with arc moves

You can enable an option that replaces linear moves with arcs whenever possible. When you filter a toolpath in this way, you specify the maximum and minimum permissible arc radius. Depending on surface topology and tolerance, a large maximum arc radius usually results in a simpler toolpath. The most effective minimum radius will be determined by both topology and machine tool requirements. A minimum radius that is too small can actually complicate a toolpath by producing many small arcs with the risk of cusps between them.

 

Note: For milling operations, you can restrict arc creation to specific planes through the Filter Settings dialog box.

Using the look ahead parameter

The look ahead parameter specifies how many points Mastercam will consider at a time when attempting to simplify a toolpath. You should consider the toolpath geometry when trying to figure the optimal look ahead value. For example, if the original toolpath has a linear motion that contains 100 different blocks and the look ahead is set to 10, Mastercam will create at least 10 different blocks for the filtered toolpath. If the look ahead is set to 50, it will create only two blocks. A too small number hampers simplification by limiting the number of moves that can be replaced at any one time. A large number will result in a simpler toolpath but may also slightly increase processing time. The same approach is used when filtering arc moves. The larger the look ahead, the more time Filtering will take.

 

---

ITHH

 

[ 10-28-2003, 08:04 AM: Message edited by: plasttav ]

[Brendan P]

Tell them to write the program!

I go thru the same thing.

Bunch a cry babies.

[mayday]

quote:

---

Bunch a cry babies.

---

Tell them to check there work very closly cause you had to manually write the code to satisfy them. thats what I do. just say HHmmm I could have made a mistake. they will get sick off that. Plus the boss is gonna see down time.

 

Put the blame on them when somthing goes wrong.

[Fig sign]

I don`t have noone !

 

I am alone

 

Iskander teh machinist==Iskander teh programmer !

[Lathe-Mill]

quote:

---

Plus the boss is gonna see down time.

---

he is always asking, why is taking that long to run that part?....i tought computers were suppossed to be faster?..

 

i replay, they just want to feel good and important by checking a 1500 lines program, the look busy you know, if they put the program in the control,set up and run, is too easy, they want to make it hard, chalenging.

 

[ 11-06-2003, 03:13 PM: Message edited by: Lathe-Mill ]

[mayday]

Tell em get outta the way, Let me show ya how its done! hey boss watch this. hit cycle start and walk away. just cover your arse ( make sure its right)

[Lathe-Mill]

 

i might do that.....j/k

 

[ 11-06-2003, 03:14 PM: Message edited by: Lathe-Mill ]

[crazy^millman]

I have not looked at a psoted program complete in over 5 years and your boss needs to get his head out of his arse on that point. I would also look at rooldie for this application been soem diccusion about real cool will put the code the way I think you want it and pretty straight foward once you do it a coulple time I have been showed its effectiveness.

 

Crazy Millman

[Müřlıń®]

quote:

---

Iskander teh machinist==Iskander teh programmer !

---

I feel your pain buddy

 

I must have a heart to heart with my boss someday......hes such an a$$.....he never gives me a raise and blames me for everything

 

 

Murlin

[crazy^millman]

So when he is talking to you is that in the Mirror Murlin. J/K

 

Yeha I know I am a bosses worse nightmare i say it like it is and say what I mean. I dont sugar coat it and dont lie so I guess that makes me a bad team player huh.

 

Crazy Millman

[Fig sign]

quote:

---

I feel your pain buddy

---

It `s not a pain .

I am sorta braggin`

It has a lot of advantages !!!!

 

I am not very easy man in life ,worse than Millman ,but I am in peace with myself .

 

Kinda I wrote the f&*#, I pressed the button is for me !

 

Iskander in solitude

 

[ 10-29-2003, 06:58 AM: Message edited by: plasttav ]

[McRae]

I have delt with difficult operators and in order to get them to buy into what I have provided them, I get them into my office and then show them the tool path running inside of Mastercam. I then post the code in front of them and show them the posted code. If there are questions on the code, then I answer them there and send ot to the machine.

 

With your operators looking thru the code line for line - get your boss to call me and I will expain to him that with every set up, people are simply wasting time. There is no way that someone (at an operator/setup) can look at a line for line program on and then say at some arbitrary point that there is a problem, chances are that there is something 1500 lines form now that will address their concerns (Tool changes and advance/retract are exceptions but with a stable post those go away).

 

In today's global competitive manufacturing marketplace, I bet that you could get rid of at least 3 people by streamlining thereby making your own company stronger and more competitive.

 

Eliminate the non-value added tasks - you are doing a good job so why are they checking something that you know in your heart to be right?

[Müřlıń®]

quote:

---

It has a lot of advantages

---

+1 yup....when I make a program I already know its going to be good....unless of course your machine tool does something wierd......

 

 

Murlin teh HEY THE TOOL IS NOT SPOSE TO BE PLUNGING THERE!!!

[John Summers]

I'm going to side with the operators on this one. It shouldn't take 15 blocks to go one-half of a degree! This amount of data is choking the machine. Where did all that data come from? (What form was it in originally?).

 

Could you make use of a cam generator?

[Reece L Gibson]

Does the control have "Cylindrical Interpolation" feature?

I know Fanuc has it and Fadal has something Similar. That shorten's the program.

[Zero]

quote:

---

It shouldn't take 15 blocks to go one-half of a degree!

---

that's what the filter is for....

 

 

quote:

---

It has a lot of advantages

---

sure does

 

[ 10-29-2003, 11:15 AM: Message edited by: Zero ]