"hybrid" roughing path?????

[prosoft]

help required to generate toolpaths for "hybrid" roughing path...... need some sample files that does the job... thanks

[Hardmill]

If none of the samples do anything for you,

You could always upload your file to cadcams

ftp site. Be sure to zip it first. Thanks

 

PEACE

[prosoft]

please help me on this????

thanks

[crazy^millman]

Hey prosoft the sample files come with your install of Mastercam if you installed them look in your C:Mcam91MillMC9Samples file and see if that helps you. If not then look at this post and see if you understand what I mean about providing us with information.

 

A Model Please

 

Hope you understand what I am trying to say. You want help be more than gald to give you help but we need more information from you to help you. If you want to type in your language I can translate is using my program to get what you are trying to say.

 

Crazy Millman

 

[ 08-26-2003, 09:12 PM: Message edited by: Millman^crazy ]

[Mick]

Heya Guys,

 

What Prosoft is wanting to know, is wether Mastercam can provide a roughing path which can do a standard OD rough pattern, but at the end of the pass "stop short" of the end of the contour, retract, and then face rough the end of the contour. The reason for this, is that a potential customer of his, is looking at purchasing Mastercam. They machine a lot of stainless steel components, and when machining the second op, if they use the above method, it removes the "waste ring" of material that is left, which can jam against the jaws, and/or hammer the insert. They find they can get really good insert life using this method. They're currently using an old version of Smartcam, that allows them to add this little move at the end of each roughing pass (its only needed on the passes at the beginning, which breal pass the face left from op1), but I've played around with sample files, and I can't find anything there that would allow it to be done (quickly)

I've uploaded a sample file under Lathe on cadcams FTP site, called ROUGH-TURNING.MC9, in which I've "mocked up" these roughing passes, by using some finish contour passes. This could very well provide the solution. Just a little time consuming to achieve it, thats all

Feel free to check the file out.

 

Cheers,

 

Mick

[McRae]

quote:

---

old version of Smartcam,

---

Even after 5 years - the old version of Smartcam lathe is much more effective for customizing a tool path. The only thing that your guy could do is to create the tool path as geometry, then use contour to do the job. This is the closest that I have come anyway. Also this gives the control required for High Temp turing paths.

 

ChrisM, Any further comment. I don't want to be the only answer for this guy.

[Mick]

Thanks for the answer Andrew. Hehe, yes, it was my opinion also. When he showed me this old version of Smartcam, and what he could do with it, I do have to admit, it had a bucketload of flexibility for its age (and believe me, it was old. This was a DOS version :/)

Anyway, I'm still pro Mastercam

It certainly was my opinion, that the only way to achieve this kind of toolpath, was to do as I had done, and create extra geometry.

 

Cheers,

 

Mick

[crazy^millman]

Well mick I am glad you explained that but how do we get what you said out of this:

quote:

---

help required to generate toolpaths for "hybrid" roughing path...... need some sample files that does the job... thanks

---

I am glad you were able to help him and if they go look at the Mitsibushi CNMG432 or WNMG432 inserts. Cant rmemeber the grade but they may find that in stainless they might allow them to get the survial they are looking for in this application.

 

That is a very cool thing to be able to do. I have sat here thinking about the Okuma, Haas, Mori, Hyundia, and Mazak Lathes I have ran and dont remember any of them having that as a can cycles or something like that. I have wrote the long code to do things like that but yeah you are right a real pian in the rear.

 

Crazy Millman

[Mick]

Millman,

 

Hehe, you dont get that out of what he typed. He asked me, and then told me later that he had put a request on the emastercam forum. I figured that he had quoted only *part* of what I told him. Put it down to inexperience on his part

 

Needless to say, thats why I jumped in and explained it a lot clearer

 

But yes, it would be a handy feature. Something along the lines of "shorten roughing contour on first (insert number passes) and finish to length vertically, or something like that

 

But for now, it looks like the method I used is the only way. Certainly seems to work.

 

I had a play on our Okuma lathes today, but you're right, there's certainly nothing in the LAP cycles to accommodate that

 

Cheers,

 

Mick

[Fig sign]

quote:

---

They're currently using an old version of Smartcam, that allows them to add this little move at the end of each roughing pass (its only needed on the passes at the beginning, which breal pass the face left from op1), but I've played around with sample files, and I can't find anything there that would allow it to be done (quickly)

---

Yet it can be done quickly and I do it in such a way.

You are talking about roughing , right .

I write a rough pass I depth only compensation to computer .

Backplot my geometry and save it .

Now i build an add-on for a center of the mill.

I replace my original geometry with a backplotted and add my add on geometry ,

change compensation type to off , add depth cuts->depth cuts order by depth and here we are !

 

[ 08-28-2003, 05:32 AM: Message edited by: plasttav ]

[McRae]

quote:

---

Yet it can be done quickly and I do it in such a way.

You are talking about roughing , right .

I write a rough pass I depth only compensation to computer .

Backplot my geometry and save it .

Now i build an add-on for a center of the mill.

I replace my original geometry with a backplotted and add my add on geometry ,

change compensation type to off , add depth cuts->depth cuts order by depth and here we are !

---

Exactly - the thing with Smartcam though is this process was much simpler and could be encorporated into a nice macro. You didn't have to have a BSc in ComSci to create that macro either...

[Fig sign]

The best program for this sort of things was an antic mac Auramill program.

It has a free machining button choosing wich meant that after selecting any contour or pocket you was able to add free hand mouse movements !

they were added to the end of that pocket or contour .

It was very CONVINIENT !

Now you can buy a c-hook for mouse machining from Camaix or use the Brian314 c-hook crlength.dll

Very useful for this purposes !

Thank you Brian !

What I miss there is no option for line -multy !

 

[ 08-28-2003, 09:21 AM: Message edited by: plasttav ]

[Guest CNC Apps Guy 1]

OK friends, here's my suggestion, use the "Direction" switch on the second page of the toolpath parameters page. You can control plunge angle as well as approach angle at the same time for entry and exit.

 

That's my story and I'm sticking to it.

 

HTH

[Guest CNC Apps Guy 1]

... and upond further reading, if the customer/potential customer wants the ability to add cutter comp to the path, just go into the "Toolpath Editor", find the point before the approach and turn comp on, find the last pass, and where the exit is (using "Direction" in conjunction with this gives clean results) turn comp off.

 

Badda-bing!

 

HTH

[Roger Peterson]

I did not look at the file so I am not exactly sure what the goal is but it sounds similar to something that other customers have wanted. The quickest solution I have come up with is to create a couple of simple lines or even points that represent the move and then use the toolpath editor and select the point right before the desired move and then add the points to create the desired move and then move on to next op. It has been quite some time since I did this but it was quite quick and the fact that I created the geo before the toolpath makes it quite easy.

 

 

HTH

[crazy^millman]

Well dont use the lathe part of Mastercam so glad you guys that do helped out on that one. I just added this one to my growing Mastercam Book cool tips from all of you. I appericate it even though I am not the one that needed it. That is what I like about this place good ideas from some smart people.

 

Crazy Millman

 

[ 08-28-2003, 10:33 AM: Message edited by: Millman^crazy ]

[Mick]

Roger,

 

If you get a chance, have a look at the file. What you suggest is pretty much what I did.

 

And thanks to all for the responses. More proof that this is one of the best Mastercam resources avaliable.

 

Cheers,

 

Mick

[McRae]

Mick,

 

Great lloking tool path. I can see the value in wanting to do this type of a machining operation to prevent packing of the rings and preserve tool life (Carbide doesn't like the tensile stress that much, and from the cursory look that I had, this will kepp them all in compression).

 

James - Check the file from the forum I can't see how the switches for leadin/out will achieve this type of motion. Perhaps you could post an example of your thoughts.

 

[ 08-29-2003, 08:45 AM: Message edited by: Andrew McRae ]

[Guest CNC Apps Guy 1]

Friends,

 

I'll show my example and put it up on the FTP this weekend so stay tuned.

[crazy^millman]

Well Darn I will not be able to see it since I dont have Mastercam lathe. How about emailing me a posted program so I can see the code and follow it that James. I appericates it in advance. Any Fanuc code will do just incase you were wondering I can follow just about any of them.

 

Crazy millman

[Mick]

James,

 

I'm staying tuned

Actually, I'm keen to see your example. Its great to see other ppl's thoughts and examples.

 

And Andrew, yes, after talking to these guys, and seeing how they program for jobs like that, I can see the benefit. Imagine how much I could have saved on carbide in the past :/

(Actually, best not to think about that..hehee)

 

Regards,

 

Mick

[Guest CNC Apps Guy 1]

Cant seem to get access to the ftp.

[Jayson Kramer]

CDC Surfcae Finish..

Is james file located on the FTP as a Zip file under the MC9 Folder..

 

So james are you using the Direction as a place to add the g41 cutter comp?

[Guest CNC Apps Guy 1]

Yes I use the "Direction" button to get myself a lead in/out line then I go into the toolpath editor, turn on comp at the X/Y move for the first pass, and then for the last pass I turn it off the move before the "Z" move. True it is a "Work Around" but that's what the Toolpath Editor is there for - to be used. I also use it for in case I have a small secion of a progrm where I have to slow the feed down, I 'll use the toolpath editor and do it. Works like a charm. Like a charm.

[Mick]

James,

 

Nice toolpath. Unfortunately, I dont think I made myself clear, but this is a lathe profile I'm dealing with

Still, maybe the Toolpath editor might allow something to be done there

I might look at it later (tho I'll need some coffee to keep me awake )

 

Cheers,

 

Mick