Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Billet roughing programs


TERRYH
 Share

Recommended Posts

       We rough a lot of parts that start as a billet of alum. and for years have used the older surface rough pocket which does a good job IMO but trying to move and use more and more of the newer high speed programs been playing with the surface high speed opti rough and don't quite think I have all the settings down yet, it ran good in verify and the total time was almost 26 mins its a fairly small part using a 3/4" button cutter, I did a surface rough pocket and the time dropped to 19 mins. I would assume something called a "high speed" program would have been faster with both using the same step over and down. Does anyone have some good info on all the required settings for the newer roughing, or know of some good tutorials. We do a lot of roughing using 3,4,5 inch high positive bull nose cutters when doing the larger billets for headliner molds. would be nice to learn something new to save time and make it more efficient. 

Link to comment
Share on other sites

I can only speak from my experience for my size of parts.

Unusual was 20 x 20 x 5 thick but average was within 6 x 6 x 4 envelope.

14mm dia MA Ford 3flt knuckle 45deg cutter with 21mm DOC with 30% stepover and S10000 F7500 (metric) and let it eat. Awesoome paths.

 

  • Like 1
Link to comment
Share on other sites

Have to be careful with the toolpath times and your backfeedrate. To get a good time use Rapid Retract for everything to see the real time in cut then switch back to backfeedrates and you will see what I am talking about. I have a part right now I have to stop every 20 minutes for an insert check, but every operation have to be checked to a fail safe and shim check and everyone of them numbered and labeled sequentially. What in another shop would be one operation for this customer is 220 operations. I have to balance the acutal time in cut with the back feedrates to make sure I have it correct.

  • Like 1
Link to comment
Share on other sites

The older surface rough pocket does a good job for what we do and depending on the size of the part which for a headliner for a car, truck can get very big especially when you have the runoff added, we typically deal with billets over 100" long 50-60" wide and up to 12-14" thick,  but with the older tool paths they only allow you to select a tool and no holder like they do with the newer high speed tool paths which is a pain in the azz unless someone knows a way to do this that we don't. we either create the tool in the stand alone editor which we don't like to do because it adds it as an assembly and clutters the permanent library, or we have been creating a dummy program that process real fast with desired tool and just selecting is when we do the actual desired tool path. which I think is stupid. 

Link to comment
Share on other sites
8 hours ago, TERRYH said:

The older surface rough pocket does a good job for what we do and depending on the size of the part which for a headliner for a car, truck can get very big especially when you have the runoff added, we typically deal with billets over 100" long 50-60" wide and up to 12-14" thick,  but with the older tool paths they only allow you to select a tool and no holder like they do with the newer high speed tool paths which is a pain in the azz unless someone knows a way to do this that we don't. we either create the tool in the stand alone editor which we don't like to do because it adds it as an assembly and clutters the permanent library, or we have been creating a dummy program that process real fast with desired tool and just selecting is when we do the actual desired tool path. which I think is stupid. 

Do a dummy drill path to set your holders for the old school toolpaths. Once the holder is set as an assembly you then can go through the tool manager in the Mill Toolpaths tab and adjust stick-out if needed. I will create a dummy drill toolpath for each tool when I am using the old-school toolpaths naming it set tool and holder dummy and ghost it. I have it if ever need to make adjustments.

  • Like 2
Link to comment
Share on other sites

That is basically what we do creat a dummy tool path to get tool and holder then create the actual needed program, and it is a somewhat easy work around just more clicks. I don't see it as a huge deal for them to simply add a holder tab to the older toolpaths when thy update stuff. BUT it seems they like adding clicks like whenever using any of the surface high speed tool paths you have to click twice to select your desired surfaces when to me it should be automatic because when selecting that tool path type you have to select surfaces why do I need to click twice to do it..............guess it is what it is and they know best. 

Link to comment
Share on other sites
6 hours ago, TERRYH said:

That is basically what we do creat a dummy tool path to get tool and holder then create the actual needed program, and it is a somewhat easy work around just more clicks. I don't see it as a huge deal for them to simply add a holder tab to the older toolpaths when thy update stuff. BUT it seems they like adding clicks like whenever using any of the surface high speed tool paths you have to click twice to select your desired surfaces when to me it should be automatic because when selecting that tool path type you have to select surfaces why do I need to click twice to do it..............guess it is what it is and they know best. 

The new controllers are that way too. At least one extra press is needed to make an offset change than before

Link to comment
Share on other sites

What kind of machine are you running in?hp wise ?Make sure you crank up your backfeedrates up as mentioned. And you can also pinch down the Micro lift to a thou or so. I also change all transitions to minimum distance not full vertical retract and I output that move to a feedrate of the max the machine can feed I agree Opti rough is better for end Mills but it can be deadly with face Mills too... I have been using one of the newer Mitsubishi adx shells with impressive results... It's a monster of a hog out tool

Link to comment
Share on other sites

I tend to do OptiRoughing with my 1" Kennametal mill 1-10 bullnose insert mill. That thing can rip through Alum like its eating breakfast. In terms of Optirough, there are alot of controls that can create redundant moves that do not make sense. Crank your back feeds up to max rapid, run the tools faster. That is my approach. I also used to hate when it would rapid up and back down to the new cut zone, but Ron is right, sometimes Z rapids are quite a bit faster than back feeding. Once you understand the controls, I think you will appreciate the new HS toolpaths more. That isn't to say "traditional" 3D paths do not have a valuable role to play.

I find using smaller tools and running them faster results in fewer restmilling ops, quicker material removal etc...obviously you want to use the biggest tool you can, but sometimes a 1" for me is faster than a 2" on a machine that maybe has limited torque or something like that.

Many ways to skin a cat

Link to comment
Share on other sites

also.. sometimes the 1" will get your program to the floor quicker than using a 2" and subsequent rest mill toolpaths

this is a valid approach for a one off part, but it's lazy programming for a production part

  • Like 1
Link to comment
Share on other sites
5 minutes ago, gcode said:

also.. sometimes the 1" will get your program to the floor quicker than using a 2" and subsequent rest mill toolpaths

this is a valid approach for a one off part, but it's lazy programming for a production part

why is it lazy programming?

Link to comment
Share on other sites
20 minutes ago, Metallic said:

why is it lazy programming?

we've got a Catia part running out on the floor right now done by a contract programmer

a 3ft x 6x x 12" thick block of aluminum that will weight maybe 20 pounds when the shooting is over.

the guy is roughing it with a 1" carbide endmill

window and cut it... took 5 minutes to program and 4 shifts to rough it

The better way is a Ø4" iscarmiil, then a Ø2" iscarmill rest rough followed by a 1" rest rough

A lot more work to program but 60 to 70% better cycle time

Link to comment
Share on other sites
15 minutes ago, gcode said:

we've got a Catia part running out on the floor right now done by a contract programmer

a 3ft x 6x x 12" thick block of aluminum that will weight maybe 20 pounds when the shooting is over.

the guy is roughing it with a 1" carbide endmill

window and cut it... took 5 minutes to program and 4 shifts to rough it

The better way is a Ø4" iscarmiil, then a Ø2" iscarmill rest rough followed by a 1" rest rough

A lot more work to program but 60 to 70% better cycle time

 that is why I said "use the biggest tool you can". My parts definitely usually arent that large...maybe ill be at 12"x12"x4", so a 1" makes more sense in alot of instances. But I agree, he probably made a fortune!

 

Link to comment
Share on other sites

I find Area rough better than opti rough for roughing out Aluminium.

The advantage with Opti rough is zig zag cut which you cant with Area Rough. I find Area rough more efficient.

Still I think both need work and you really need to watch the toolpaths on the machine to see that they are not the greatest in rapid metal removal.

Link to comment
Share on other sites
15 hours ago, DavidB said:

The advantage with Opti rough is zig zag cut which you cant with Area Rough. I find Area rough more efficient.

If only they had zig zag in Area Rough. :D   I've said that to myself more than once. 

I wish that the "keep tool down" controls worked better as well.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...