Highfeed help

[wildcat99]

I have 3 aluminum mold inserts to cut on our router next week and would like to try out the Highfeed option or at least the Adjust Feed on Arc Move. There will be a mix of both 3ax and 5ax toolpaths. I will have just enough time to setup, cut and get the parts off before the machine is turned back over to Production for trimming. I haven't cut a test circle for the cornering acceleration values in Highfeed and don't know if I will have time, but I have ballpark values, probably conservative, that might work.

 

The aluminum we've cut in the past has turned out fine, but I have an opportunity to use Highfeed and would like to see how it works with our router. I like the idea of adjusting the feed when needed, reducing chatter in the corners, etc without keeping a constant hand on the feed override knob.

 

My questions:

This is from the Help menu

quote:

---

For examples on how to use the Highfeed machining, see the HFAPP_V9.DOC file in the MCAM9CHOOKS folder

---

I don't have this file on my PC anywhere, where can I find it?

 

What values if any should I change in Highfeed, especially in the feed rate smoothing options? Or should I leave all at the defaults?

 

Is Highfeed too much to set up correctly in this short amount of time? Should I just use Adjust Feed on Arc Moves now until I have more time to experiment?

 

I don't have any experience using these options so I'd appreciate advice from anyone who does! Thanks.

[Don S at Barefoot CNC South]

What is your email address

 

Don S

[Dennis at CAD/CAM Consulting]

If you only want to decelerate into and accelerate out of corners you only need to set the finish pass options. Highfeed will only reduce the feedrate from the programmed feedrate. Make sure you set the minimum feedrate to something acceptable. I usually adjust the "Look ahead" to about 200% and turn on the "Accelerate to smooth feedrates and go with the default setting of about 2%. I usually change the "Maximum feedrate change per block" to about 5% and the "Recombine segments" to about 4%.

 

The most important thing to be aware of, It does not function correctly if you turn on cutter comp. In v9.1sp2 and 9.1mr0304, If you set the compensation type to Control or Wear or Reverse the results will not be what you would expect. Usually mostly it does not decelerate into the corner. But it does drop the feedrate at the corner and accelerate out. Use "Computer" comp for best results.

 

If you want to cut at 100 inces per minuet and slow down to 50 or something in the corners just program the whole thing at 100ipm and set the "Minimum cornering feedrate" to 50. The look ahead is the distance from the corner at which the machine begins to slow down.

 

Something else. The operation is locked after running highfeed. If you need to change it you have to unlock it, make your changes, regenerate and run highfeed again.

 

To really gain optimum performance you need to cut the test circle. If you can't do that then just backplot with the "Show Coordinates" and "Verbose" mode turned on and you will be able to see the feedrate changes as you step thru the program. You can unlock, regen and Highfeed again until you get what you wanted.

 

Hope that helps,

[Paul_RagotCADCAM]

Wildcat99,

 

This file comes with the V8 CD. It is not on any V9 CD as far as I know. It has not changed since V8.

 

Paul

[wildcat99]

Don S:

My email is [email protected]

 

Dennis:

Thanks for the suggested settings. I always use "Computer" comp here. I will do what I can to get the test circle cut. The test circle, from what I understand, is cut once at a low feedrate for accuracy then recut at gradually higher feedrates until it gouges into the sides produced by the first cut? Or do you start over with a new block of material at each feedrate increase until the circle is out of round or measures incorrectly?

 

fennex:

Thanks, I'll check V8 at work tommorow.

[Don S at Barefoot CNC South]

Wildcat99

Sent you an email with a doc on high feed.

 

Don S

[Mike Whitten CAD/CAM Contractors]

Wildcat99,

 

I would like to add my 2cts on this one.

 

The Highfeed option is a very nice feature and it will help you out mostly if your machine does not have any type of "Look Ahead" funtion on your control.

 

The biggest thing about the Highfeed option is that you must know exactly what you want before you can dial in all of the parameters. What I did was have three different "machines" per actual machine.

 

IE:

 

Haas #1 (servo lag limit 1 large amount lag)

Haas #2 (servo lag limit 2 medium amount lag)

Haas #3 (servo lag limit 3 no servo lag)

 

With some time you can define the levels of servo lag to an actual amount.

 

This way you can push the machine to the absolute limit depending on the tolerance of the job and other requirements.

 

You will love it once you get some time in on it. Only thing is, you will just want a machine with more feedrate!

 

Thanks,

 

Mike

[wildcat99]

Thanks Don S and fennex, I'm reading through the Highfeed Apps Guide now.

 

To get everything dialed in, it looks like I need to cut the test circle and get the Material Removal Rates defined as close as possible. For MRR I'll start with values from past aluminum jobs that pushed the router pretty hard, but still cut OK. Does this sound reasonable?

 

Also, I will be using STL files to define the stock. After running Highfeed on all operations in one plane, do I need to create a new STL file to use with Highfeed on operations in another plane?

 

I also use G51 Look Ahead at the control - a xxxxor 8055M - if that makes any difference.

 

Thanks to everyone else for all the suggestions so far. Keep 'em comin if anyone else would like to share their experience with highfeed.

[Mike Whitten CAD/CAM Contractors]

Wildcat99,

 

I am on a hot job and must go soon So here are a few things to consider.

 

I am not at all familiar with the xxxxor look ahead function but on some of the machines that we have, the look ahead takes care of all of the servo lag. IE: you do not need highfeed to slow down for servo lag reasons. You must find this out by doing some testing, cutting a circle or whatever.

 

If you are using the WCS, you can leave the model alone and just use one STL file. IF not then you must use a different one for every op.

 

Mike

[wildcat99]

From what I understand our machine has very low servo lag/following error. So I would be using highfeed to slow down in corners and to speed up when cutting little or no material for example. I'm sure our machine can accurately take a sharp corner with little or no servo lag, but this is too fast when actually cutting because of chatter, flexing etc.

 

In our xxxxor manual for G51 Look-Ahead it says:

quote:

---

"Usually a program consisting of very small movement blocks (CAM,digitizing,etc) runs very slowly. With the G51 feature, high speed machining is possible for this type of program.

.

.

....because the CNC has to analyze the machining path ahead of time (up to 50 blocks) in order to calculate the maximum feedrate for each section of path.

The programming format is: G51[A]E

 

A(0-255) Is optional and it defines the percentage of acceleration to be applied. When not programmed, the CNC assumes the acceleration value set by machine parameter for each axis.

 

E(5.5) Maximum contouring error allowed.

 

Parameter "A" permits using a standard working acceleration and another one to be used when executing with Look-Ahead.

 

The smaller the "E" parameter value, the lower the machining feedrate. When operating with Look-Ahead it is a good idea to adjust the axes so their following error (lag) is as small as possible because the contouring error will be at least equal to the minimum following error....."

---

We normally turn G51 on at the start of every program to smooth out the incremental, stutter-step type movements. I might have to turn this off when using highfeed, I'm not sure.

 

Should Highfeed, Adjust Feed on Arc Moves, Filter and Look-Ahead at the Control all be used simultaneously or if you use one don't use the other for example?

[Mike Whitten CAD/CAM Contractors]

Wildcat99,

 

I believe you can use all of these functions simultaneously. Here is the thing. The Look ahead (G51) with the error control setting is one of the best things on the market. I would spend some time testing all of this stuff so that you figure out exactly what you want.

 

Mike

[Mike Whitten CAD/CAM Contractors]

Wildcat99,

 

I end up not using Highfeed as much on our look ahead controls. I use them mostly on our older machines.

 

Mike

[wildcat99]

quote:

---

If you are using the WCS, you can leave the model alone and just use one STL file. IF not then you must use a different one for every op

---

I'm not using the WCS so I will be using different STL files. How do you save an STL file in Verify with ops that are not in the top plane? I get this "Warning TrueSolid Turbo:3-axis moves in top view only".

 

With a little help from my dealer, I was on my way saving the 1st STL file in Verify with my 1st 3 ops in the top plane. The problem is the next 6 ops in a non-standard plane don't show the material removed in verify and can't be saved as the proper STL.

 

Can Mastercam save STL files representing partially machined stock or do I need to model each in Solidworks for example and import in for stock?

 

Thanks for your help

[Mike Whitten CAD/CAM Contractors]

wildcat99,

 

You can not use turbo when your ops are not from System view top. I have asked for this many times but I do not think it will come soon.

 

The "work around" for this is to just change Display control settings in Verify. You can change your moves/refresh up to 100000. This is not as fast as turbo but it allow you to Verify at a much higher speed than seeing the Tool.

 

If you are using Five axis ops, you must have "Five axis Verify" to save STL as you must run in True Solid mode. I had this problem also until we purchased the "Five axis Verify" Option.

 

It works great.

 

Is this the Info that you need? Did I cover it?

 

Mike

[wildcat99]

Mike:

Yep that did it. From the little Help popup it made it sound like you had to run in Turbo to save an STL.

 

Yeah I use 5-axis ops often and also found that Verify can be deceiving when you can't use TrueSolid, let alone not being able to save an STL.

 

5-axis Verify

Can I get this from my dealer?

 

Thanks, you've covered everything very well. I appreciate the time you've taken to help me learn something new.

[Mike Whitten CAD/CAM Contractors]

Wildcat99,

 

quote:

---

5-axis Verify

Can I get this from my dealer?

---

Yes, I believe it is a must. All it takes is one expensive scrap part and it would cost far more than the software would have cost. It is fairly priced for what you get.

 

quote:

---

Thanks, you've covered everything very well. I appreciate the time you've taken to help me learn something new

---

You are very welcome.

 

Mike

[Rekd™]

quote:

---

The most important thing to be aware of, It does not function correctly if you turn on cutter comp. In v9.1sp2 and 9.1mr0304, If you set the compensation type to Control or Wear or Reverse the results will not be what you would expect. Usually mostly it does not decelerate into the corner. But it does drop the feedrate at the corner and accelerate out. Use "Computer" comp for best results.

---

Thanks for the help!