Sign in to follow this  
Followers 0
Hcarte

Legacy toolpaths vs OptiRough for Die and Punch work

26 posts in this topic

We would like some input on some of the new toolpaths. We have been trying to make them work with the type of parts we make and we just cant seem to get any where with them. I have attached a die we made it took just over 15 hour to machine it. The part was cut out of 7.00  A36 plate with a CNC torch.  We use Sandvik 210 high feed cutter to rough with. Then we use a sandvik 200 cutter for Restmill and Parallel passes. We use a 1.0 insert ball mill for finishing, after that we will do some leftover toolpaths  with smaller tools.

 

 I had to zip the part it is 25MB

Thanks

Howard

 

post-20091-0-01658100-1487268141_thumb.png04312-die-2ND-SIDE-TEST-MASTERCAM.ZIP

3 people like this

Share this post


Link to post
Share on other sites

What toolpaths can't you get to work? 

Share this post


Link to post
Share on other sites

Jeff,

I keep reading that people quite using the legacy toolpaths because the new Dynamic and Opti stuff is so great. I just can see  how a end mill to rough a part like this is better than what we are doing.  I think Dynamic and Opti  is another tool in the tool box, but for the parts we do they are not a good fit for us.

Share this post


Link to post
Share on other sites

Sounds like much of what is good and easy with the new toolpaths was flame cut off before you got the material. Seriously, new paths excel at machining a shape like that from rectangular stock.

 plus if you are using high feed sandvik stuff, i'd have to agree that legacy z-level strategies would be hard to beat.

1 person likes this

Share this post


Link to post
Share on other sites

Jeff,

I keep reading that people quite using the legacy toolpaths because the new Dynamic and Opti stuff is so great. I just can see  how a end mill to rough a part like this is better than what we are doing.  I think Dynamic and Opti  is another tool in the tool box, but for the parts we do they are not a good fit for us.

That's quite possible.

Your part is pretty good size, maybe others with experience in programming large molds like yours can help you better than I can.

My parts are a LOT smaller than yours. 

Share this post


Link to post
Share on other sites

Area rest rough will have the exact same cycle time, feed rates being equal, as rough pocket but the calculation time will be slightly better and the system will not be frozen while its crunching.

You could prolly run a 3" sandvik @4000rpm in A36, which has nothing to do with MC, just sayin. If you were to bump your feed rate a commensurate amount up to 350ipm, the rounded/smoothed opti paths would be easier on the machine and would also likely run closer to the back plotted cycle time of 1hr.

Share this post


Link to post
Share on other sites

Area rough from a stock model of your burnout will cut nice on this with highfeed mills. And some corner rounding in your parameters and the machine really smooths out. Draw a big xxxx window around it for stock and reference the stock in your toolpath. You can then approach from the outside or stay inside. You can also holder collide check with the new paths. 

Share this post


Link to post
Share on other sites

we have been using opti ruff with iscar fast feed with great successes you are always in a climb mill state with controlled engagement so spindle load is constant and tool life is great! way faster then the old trusty surface rough pocket. you can go max depth of feed mill and max chip load, play with step over until you like the way its cutting.

Share this post


Link to post
Share on other sites

Anyone else having this file lock the computer up?

Share this post


Link to post
Share on other sites

I think you have run into one of those not always situations. I threw a Opti-Rough toolpath at your part. In this case using the tool you are using the way you are using it you might have the best way to machine that part in Mastercam. You start thinking about using something different like a 7 flute tool maybe 3/4 in size then we can have a different conversation, but like you are I can't see where the Opti-Rough will do better than what you have worked out with Surface Rough Pocket. I would like to hear with someone from CNC software would say about this.

 

I used the same step down and step over and got 8 hours with Opti-Rough and see you are getting about 3 with surface rough pocket. Excellent work sir.

1 person likes this

Share this post


Link to post
Share on other sites

I got it down to 3 hours and change

The controlled radial engagement and 60% step over would probably be easier

on the spindle but I couldn't beat the original time

Share this post


Link to post
Share on other sites

2:45 @82% stepover and 100ipm


 

1:00 @350ipm

be brave :smoke:

1 person likes this

Share this post


Link to post
Share on other sites

2:45 @82% stepover and 100ipm

 

1:00 @350ipm

 

Give Surface rough pocket the same feed rates and compare apples to apples.

Share this post


Link to post
Share on other sites

Give Surface rough pocket the same feed rates and compare apples to apples.

yep. Post #6 :-)

Pretty much the same in the computer. On machine a little smoother, IMHO.

 

edit: first crack at opti, was 8hrs too.

Share this post


Link to post
Share on other sites

I use a lot of high feed cutters from 2.5 to 4in on large parts and the area paths are always faster. TBH I'd call yours a small part. You might consider a plunge cutter. In some cases you can wear it out by plunging with the right cutter. Like everything else, it's up to you to decide the most efficient and cost effective way to get the material out. In CAM I could make a path faster with a 1/8in ball mill but we all know the difference between the real world and how it looks on the screen. Your roughing looks really good, all the time in that part will be in the finishing.

Share this post


Link to post
Share on other sites

I would like to look at this file but it will not open for me can someone save it in a different orientation with the part level turned off or something...I have never run into this before i let it try to open for 30 minutes and the little 

mastercam giff with tool cutting just keps going ang going...

Share this post


Link to post
Share on other sites

Thanks dude that one opened right up....

 

I am thinking my video card pushed this popup underneath and I could not get past this...

 

 

post-5941-0-40600200-1487351893_thumb.jpg

Share this post


Link to post
Share on other sites

yep. Post #6 :-)

Pretty much the same in the computer. On machine a little smoother, IMHO.

 

edit: first crack at opti, was 8hrs too.

 

gotca.

1 person likes this

Share this post


Link to post
Share on other sites

There are more to the new toolpaths than just opti rough...

 

There are many reasons why the new toolpaths are better than the legacy.

 

I used to think as you do. I owned a forging die shop and machined shapes like this for a couple decades and can

say that the new toolpaths run better, leave less to polish, are easier on your machines, cause one to think in a

new direction and end up and save your shop time and money.

 

Observe the motion between the new dynamic toolpaths I have done vs the legacy.

The transitions are smoother, there are no little weird peices that have to be edited out, they are just better.

 

This part came out in just under 10 hrs..

But the roughing was about the same.

 

 

Time saving was all in the finishing and approach.

 

post-5941-0-25021300-1487423658_thumb.jpg

 

 

https://www.dropbox.com/s/ofkj2ralaa1ref1/MurlinTEST-MASTERCAM.rar?dl=0

Share this post


Link to post
Share on other sites

Thanks all of you for looking at this part and all of your responses. I'm sure I'm going to make myself look fairly

unintelligent with this next question, but Murlin, is this Mastercam File You have pictured in your post

saved in a format in which we can open it up and look at how You have set up the new tool paths? I am

new to the site, and am not aware of how these files are normally passed back and forth.

     If it is not saved in a format we can open it in, can You do so? I am very interested to see how You

have set up these new tool paths.

 

Thank You,

 

Steve

 

 

 

 

post-5941-0-25021300-1487423658_thumb.jp

 

 

https://www.dropbox....TERCAM.rar?dl=0

 

2 people like this

Share this post


Link to post
Share on other sites

It is a 2017 file. Anyone who has 2017 can run it.

Share this post


Link to post
Share on other sites

He is winrar for zipping his files. It is a zip utility that is like winzip. Normally winzip or even windows can unzip if you give them the association to do so.

 

Steve welcome aboard and why the site is the best Manufacturing site I am aware of in the United States. They are other ones, but this topic is what makes the place such a good site. Everyone excellent work going above and beyond.

1 person likes this

Share this post


Link to post
Share on other sites

Thanks, I figured out how to retrieve the File. I didn't know

 

an .rar File could be unzipped.

 

Steve

Share this post


Link to post
Share on other sites

Steve welcome aboard and why the site is the best Manufacturing site I am aware of in the WORLD. They are other ones, but this topic is what makes the place such a good site. Everyone excellent work going above and beyond.

Small correction there Ronaldo...

:D

6 people like this

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now
Sign in to follow this  
Followers 0

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us