High Feed Machining...MAJOR PROBLEM!!!

[ILv2Rk]

Ok guys here is the problem.

I have a 3-D Surface HST (Area Surface) toolpath which I have ran through Verify and and Vericut and everything looks good.

Now we want to incorporate the High-Feed process to speed things up and to cut down on tool breakage in tight corners of mold cavity.

This is the first time I have tried to use the high feed deal so I did extensive research on it and we did the machine test and I have set the parameters in the machine settings in Mastercam.

 

After applying the High Feed to the toolpaths I re-ran through verify to check it out....GOOD THING....because now there are places where the tool has gouged into and past what will be the finished surface.

 

Desperate for help, got the man breathing down my neck on this one.

 

Jeff

[crazy^millman]

Go back and make sure your STL if using one is still good. Make sure your Check surfaces are still there. Make sure all your drive surfaces are still there. If all else fail redo the toolpath from scratch using all the parameters you were using. either write them down or take screen shots of them.

 

HTH

[ILv2Rk]

If I unlock the toolpath and regenerate it the resulting toolpath is good until I add the High-Feed conversion to it and then it undercuts.

 

I was originaly not going to rerun it through verify because all of the documantation says that High-Feed does not change you X-Y-Z moves it only changes the feedrates but this however is not the case.

[Mike Whitten CAD/CAM Contractors]

I would re-check as Millman said first. You may then want to try "finish only" This will at least allow you to slow in the corners.

 

I have used it many times on HST with incident. I normally just use "finish only" to slow in the corners.

 

Thanks

[Colin Gilchrist]

Hi Jeff,

 

I've haven't had the best luck with High-Feed in Mastercam. I've had really good sucess with the Opti-path module in Vericut. The best thing about Vericut is it runs your acutal G-code, and it really doesn't change the path your tool runs...

 

You might be able to get CGTech to run your code through Opti-path as a demo for you, or you might be able to pay them to optimize the code...

 

Just trying to help here, I'm not sure that High Feed will give you what you want on the HST toolpaths...

[Mike Whitten CAD/CAM Contractors]

Just a thought. It may be due to the filtering. I didn't think of that one until now.

 

Jeff, how is the filtering in the HST set up?

[ILv2Rk]

Michael, In that particular toolpath the filtering is turned off with a total tolerance of .001"

[ILv2Rk]

Colin,

 

We have Vericut but we do not have the Opti-path module YET. We are looking into it though and have gotten a quote from them and CGTech is pretty proud of that module. It cost the same 10K for that module as it does for the main verification module. We are now trying to justify buying a seat of it. So you have had great results form it?

[Mike Whitten CAD/CAM Contractors]

I would say that the safest thing is to use the Vericut as Colin mentioned. If you buy it that is.

 

I am thinking that this is an Area Clearance toolpath. If yes and depending on your current situation, you may want to filter with arcs at a much looser tolerance, about 20% of stock left.

 

You will still be able to Verify in Vericut to check for a gouge.

[gcode]

Are you running the high feed toolpath through Mastercam Verify or Vericut..

If you are getting gouges in Vericut, it may be

rapid motion..

Mastercam sees rapid motion as straight lines..

most machines don't..

The gouges may be dogleg rapids into the walls

of your part.

Try forcing G01 rapids in high feed.. then they

will be straight motion and may eleiminate the gouges.

[Colin Gilchrist]

Hi Jeff,

 

I've had great results with Opti-path, and there are many different optimization strageties that are available when you use it. Much more powerful than High-Feed will ever be. It works on the G-code too, which Mastercam won't do in the forseeable future anyway.

 

See if you can get them to run Opti-path on your code as a demo...

 

Then they can send you the optimized code and you can run it in your copy of Vericut to make sure it is still gouge free...

 

Gcode is also right about not using any Rapid moves with those HST toolpaths.

 

I always use the "shortest distance" option, but force the toolpath to output feed moves at a high feedrate. This will ensure you never get dogleg rapid moves, and the machine moves in exactly the path you want.

 

For Opti-path, I see an average of 20-35% time savings, but it really depends on your roughing/finishing toolpaths. I've seen some jobs where we saved over 50%...

[YoDoug®]

+10000000 on the Opti-path. It will pay for itself in no time. We used Opti-path on a series of 26Rc 416 SS parts in our production shop. The savings results on those parts alone will save $4000/year of machine time and thats just 3 part numbers out of 500+ we machine every year.

[ILv2Rk]

Thank you so much for all of your input, I will implement these techniques and follow up with results.

 

You guys are great.

 

 

Jeff

[Colin Gilchrist]

Jeff,

 

If you do decide to get Opti-path, shoot me an email and I can give you some pointers that will help get you setup. Did you do your Vericut machine and control files in-house, or did you purchase them? Sometimes you can get the accel/decel parameters from your machine builder and make your opti-path code even more effecient.

[ILv2Rk]

Ok guys,

To much avail I have tried all these suggestions for getting my toolpaths to work and just when I thought I had it it seems worse than before.

I used the shortest distance option and forced it to output a high feedrate, I turned on my filter and set it up for 2-1 with a total tolerance of like .001" and still I get gouges.

It seems to work fine till it gets near the bottom of the cavity and then on a helical entry move it lows right into the walls as if there were no drive or check surfaces at all.

 

 

Colin,

You've got mail!

Jeff

[Mike Whitten CAD/CAM Contractors]

Hello Jeff,

 

I am sorry to hear of the bad news. Could you please let us know if the issue is showing up in Backplot and Verify.

quote:

---

It seems to work fine till it gets near the bottom of the cavity and then on a helical entry move it lows right into the walls as if there were no drive or check surfaces at all.

---

Thanks,

Mike

[hot_chip]

I am looking into starting to use the highfeed optimization in mastercam, and I was wondering if anyone had some guide lines they like to use for setting the maximum feed rate. So far I'm thinking about setting the minimum feed rate to manufacture specs, and setting the maximum feed rate by 25% more.

 

Any thoughts or advice about this? I would really appreciate it.

 

Thanks

[crazy^millman]

Look at Chris Rizzo's thread and chart for Highfeed machining and think you will find it has a lot of information in that thread that will be helpful. Remember it is about the percentage of chip load and never be afraid to bury the tool. By keeping the axial load lower you can feed it harder. Seen some very impressive speeds and feeds done using these methods.

HTH

[Müřlıń®]

Sounds like your post might be leaving out some plane changes on circular blocks.....when it processes all those federate entries. Or maybe its just not formatting them properly.

I had a control that required the plane change to be on a line by itself. Sometimes the post would put them in a g01 block and it would gouge.

 

Oh wait it could be in the nci...dont those HST still have looping entries that require plane changes when arcs are enabled?

 

Might try turning off arcs. That is the only thing I could think of that would cause gouges without changing any of the numbers.

 

I had some really good luck with the highfeed option on the legacy paths.....