STOP ME FROM SHOWING STUPIDITY!

[jenks]

This is basically a lathe question.

 

I have a problem that has bit me several times and you would think I could remember how to prevent it by now.

 

When using a reverse boring bar I keep forgetting that there is a portion of the bar sticking out in front of the point of the tool. So, when I assign my enter and retract points I make them too close to the stock, and bingo we have a crash possibility. So far I've been lucky, and one of us has caught the glitch. But, my luck can't hold out forever.

 

Is there any way I can put a message(note if you will) into the tool description that reminds me to allow for the excess length?

 

I've made a "band-aid" fix, but some of you may have a better idea. On the parameter page of the tool, on the TOOL NAME line, I added "check overhang". It ain't pretty, but it gets the idea across.

[Müřlıń®]

you could name the NCI file....Addmorelgth or sumpthin like that ... The program name would come up on the CRT.

 

You can also insert text but someone else would have to help with that...

 

Murlin teh always a workaround...

[crazy^millman]

Well I would think you could put a check in your post that is the zout vaules is less than .05 then output this text in the post something like this:

code:

---

if zout > .05,

[

(MACHINE WILL CRASH)

(SET YOUR RETRACT POINTS)

(BIGGER TO KEEP FROM CRASHING)

]

---

I hope that helps and hope that works.

 

[ 03-24-2004, 10:15 PM: Message edited by: Millman^Crazy ]

[M. Anderson]

Jenks,

 

If I understand this correctly -

 

When you use a reverse boring bar the part of the bar that is in front of the insert tip is what you are worried about hitting the part on entrance and exit of the part?

 

It is not really a tool overhang issue - but the part of the bar in front of the cutting point of the insert?

 

If that is not your problem don't pay attention to the following:

 

1st - are you using a boring bar from one of the supplied lathe tool catalogs? If you are - Great!

 

2nd - if you are not using a pre-defined bar from one of the tool catalogs in Mastercam - have you TOTALY defined the bar? You MUST define the entire bar (leading part and all) and include the insert for what I am going to tell you to work.

 

When you have the bar defined, Correctly and Totaly, Mastercam will automaticaly compensate for the leading part of the bar.

 

To make this occur automaticaly in Mastercam - go to your operation in your program that is using this bar - click on the "Parameters" of that operation.

 

That will open that operation as if you were going to edit something.

 

The tool you selected will be highlighted on the "Tool Parameters Tab" - LEFT click on the tool you selected.

 

The tools parameter page will come up - go to the "Parameters Tab" for that tool. Down at the bottom of that page is a "Tool Clearance..." button - press it.

 

A "Lathe Tool Clearance" screen will come up.

 

Press the "Scan Tool Geometry..." button - then another screen will come up and should show some numbers for tool width, height and clearances.

 

Press - "Select All" and then "OK".

 

Now the bar is properly defined in Mastercam!

 

So - NOW - Mastercam knows there is part of the bar infront of the cutting point on the insert.

 

Continue to click "OK" until you get back to the "Operations Manager" - then regen the operation - now backplot the operation and check the clearance.

 

I do this type of operation quite often - never have I had any problems doing it this way!

 

The main thing is the boring bar has to be defined for Mastercam to realize that part of the bar is infront of the insert's cutting point.

 

Post out one of your operations before you change it - then post it afterward of doing this - see what the Z location change is - it should be the amount of the leading edge on the bar!

 

I can send you a test file showing this (in version 8), if need be.

 

Hope that helps - and you can follow this?

 

Later,

 

Mark Anderson

[Nominal]

Yeah, what mark said.

I do reverse bores all the time.

Fortunately I've found these tools in the catalogs supplied with mastercam. I find it very difficult to define my own holders and tools in mc lathe. But thats probably because I haven't been taught by anyone and I usually don't have time to do it anyway. Aside from that I believe you'll have to define your stock and use recognition even if you find the right tool in the catalog. Someone else can confirm this.

[Gorn]

Nice post Mark. I was just going to say draw the bar to scale in Mastercam and its all good from there. Guess that is why I am not a teacher.

[pno]

M Anderson has totally right. I use custom tools in MC for a lot of boring bar including reverse bar,for standard or custom tools and it's work very good if you use corectly clearence and stock recognition.

[jenks]

Thanks guys.

 

I am using the supplied bars. No custom tooling at all. When the tool is defined, it does show the point back from the front. I guess Mastercam just doesn't recognize the little bit sticking out in front of the tip.

 

It is just that I always start my tools .100" off of the part. The point is then read at the tip of the tool, which is back from the end. It is this habit that gets me in trouble.

 

I did stick a note on the tool description and it now draws my attention to the fact that I have to allow more for clearance.

[M. Anderson]

Jenks,

 

I guess, I just don't understand your problem?

 

I run my start point at .025 off the part most of the time - I even run my reverse boring bars the same - if the bar is properly defined and your stock is defined in the job setup screen - Mastercam "WILL Automatically" compensate the bars movements to allow clearance for the leading part of the bar and not crash it into the part or the stock. I do this on about 10 different parts every month.

 

You do not have to allow more clearance!

 

Even if you are running one of the bars selected from one of the supplied catalogs - you will most likely still need to define the bar as listed above. Then save the tool back to the library.

 

Maybe I just don't understand your problem?

 

Sorry - but that is about the best I can do!

 

Contact your Dealer - maybe he can show you what I am talking about the next time he comes in.

 

Later,

 

Mark Anderson

[Jimmy Wakeford from Barefoot CNC]

Jenks

Are you defining the stock in job setup? If so you should be getting a warning atleast. Otherwise it will take your job setup rapid clearance and apply.(V9?)

 

Mark,

Your up late writing long posts...Did your wife get you some viagra? Or have you started selling Mastercam?

[M. Anderson]

Jimmy,

 

Up with a damn headache!

 

Besides, I am just trying to keep up with you!

I see some of your posts a 2 and 3AM in the morning!

 

See if you can figure out what Jenks is doing - I do this all the time with no problems or need for extra clearance??? I am lost!

 

Selling - Naw, Allen would not give me a job!!!

He just wants me for my money!

 

VIAGRA - I am not that old yet!!

 

Ask Allen about his MOTEL stay in Oak Ridge - next time you talk.

 

Later, this monitor is killing me.

 

Mark Anderson

[Jimmy Wakeford from Barefoot CNC]

Mark I think defining stock will solve it.

See ya

[jenks]

I always define the stock. But, defining the stock can cause other problems that I won't go in to now.

 

I think it is operator error(myself, because there is no one else to blame).

[Jimmy Wakeford from Barefoot CNC]

jenks

Why dont you put the file on the ftp. I will take a look at it and see if we can figure out whats up wid dat.