Can I Keep the Tool Down in this part?

[Reko]

I am surface/restmill roughing this part.

 

http://i610.photobucket.com/albums/tt185/MCReko/n3.png

 

Problem is, it is too big for the travel in my "Z" axis. I have to use 2 tools. The first tool roughs it down about half way, then a second tool (which CAN NOT retract above the top surf) completes the part down to the bottom.

 

Question #1 is, how can I force the tool NOT to retract above the part?

 

Question #2 is, will the rapid movements avoid crashing into the walls?

 

Thanks, in advance, for any help or suggestions :>)

[Colin Gilchrist]

If that is the case, I would try and only use the HST toolpaths. There is a retract option for "shortest distance" and you can set it to ouput all "rapid" moves as a feed move. I highly recommend this. If you use rapids inside the part, you risk a "dog-leg" rapid move destroying your part.

 

For Question #1: you might have to take your part model and make a copy of it, then "cut" the top portion off. That way the toolpath won't "see" that portion of the model and try and force a retract. Make sure you use a containment boundary. You might also try using "Reference points" to give the toolpath an exact starting and ending point.

[Ron Branch @ Verisurf]

Cut depths in any of the standard surfacing toolpaths will do what you are after since the is a basic shape and the part gets bigger at the top you should be fine. I would set my retract, and clearance to the place you want be in Z with the tool. If you want to make sure it does not give you problem you could use a point toolpath before and after the operation which would put the tools inside the part. Also do not forget about reference points in the operations they can serve the same purpose. What I will do with point toolpaths is back plot the operations then save some of the geometry then use the start and end of operations to make my point toolpaths align with the surfacing operations when doing deep cavities to make sure nothing goes crazy on the machine.

 

HTH

[Code_Breaker]

This is only one way that I do it:

 

Under Linking Parameters

 

Clearance ==> checked

Use clearance only at the start and end of operation ==> checked

Retract ==> checked

value .2

incremental ==> check

Feed Plane value .1

incremental ==> check

top of stock value 0 (same as geometry depth)

incremental ==> check

Depth vaule -2.0 (distance from top od stock)

incremental ==> check

 

 

I you are doing the same geometry in two level or tools, then top of stock will be the distance from the geometry and/or last distance of first cut.

HTH and is clear ...

[Josh T™]

Reko,

 

What type of machine/control are you making this part on? The reason I ask is for your rapid travel type. Do all of your axes arrive at the same point together or do they take the shortest point? When using HST with minimal clearance I have ran into issues with machines that go shortest point. In MC they verify great but on the machine it's a different story.

 

EX:

Our Hermle C40u rapids/feeds in vector moves. If we tell it to rapid to X0 Y0 Z1. A90. B180. it will make a straight line vector move to that point.

 

On the other hand...

Our Haas VF3 will move as fast as it can in all axes but they will not all arrive there at the same time. Which ever axis is closest will arrive at the destination 1st.

 

This info makes a huge difference when using minimal retacts and safety zones. I'm just about to the point of not programming HST paths on the Haas because of this issue.

 

Use your best judgement when picking toolpaths and really know your machine. This has bit me in the a$$ several times.

 

HTH

Josh

[KalCam]

I use Metacuts to edit the NC, especially if the part has a ton of surfaces which makes regen time crazy long. Place the part negative in z with a known max value positve in z and just keep editing/verify until it fits.

[Colin Gilchrist]

Josh, try using the "minimum distance" and setting the toolpath to output a feed move at your machine's maximum feedrate (make sure you program to the lowest max value if your axes don't have the same max feed value).

 

The reason I learned to do this is on a Haas. I was machining a cavity with the head tipped over (3+2) and the rapid retract doglegged right into one of the walls. Scrapped the part and broke an expensive endmill.

 

I've also taken to turning off "rapid retract" and putting in a retract feed value. Much safer this way...

[Reko]

Guys,

 

I just want to let you know all of your information was very valuable. Thank you all, for posting. I love having options and everyone adding to the conversation has helped immensely.

 

A few questions to expand on, if you don't mind;

 

Colin,

What is "HST" toolpaths? I'm currently using Surface/Rough/Restmill with an STL representing the stock because it is a casting with about 1" of stock on it.

 

Josh,

I run a Reko Gantry Mill with a Heidenhain controller. It is the first machine I have programmed for, that does NOT "dog-leg" in rapid. All axes arrive at the same time.

 

KalCam,

Coincidentally, I just loaded a trial version of Metacut yesterday. I'm not sure the owner will buy it. Do you like it?

I haven't gotten around to using it yet and that is why I asked this question on this forum. I'm really nervous about running the bottom portion without knowing for sure it is safe. At my last job, we used to run the part in a block of wood and verify it that way. The owner did not like us using verify or any type of verification software. He saw it as a waste of time. Now, the parts I work on are so big, I don't have a choice but to verify the program. This part's biggest radius is 64" (yes, over 5 foot) and weights around 30,000 pounds... huge! The last thing I want to do is crash, so verifying my toolpath is essential.

 

Again, thanks for everyones help and Happy Thanksgiving!

____________________________

MasterCam X4 MU1

Mill Level 3/Solids

Dell Precision T3400

Intel Core Duo CPU 2.33 GHz

2.33GHz,2.00 GB RAM

Windows XP Pro SP3

NVIDIA Quadro FX 570

[Thad]

HST = High Speed Toolpaths. You should see the option in the list of available toolpaths.

 

Where are you at in MI, Reko?

 

Thad

[Reko]

Thad,

 

What is the advantage of HST over normal surfacing? And, can I use an STL to define the stock?

 

BTW, I'm in Mid-Michigan right now. Used to work in Auburn Hills and Madison Heights too. Both of my stints down south were short lived, I like it up North better :>)

[KalCam]

Reko,

Metacuts gives good bang for the buck, just cutting wood/urethane patterns here but clean code is everything. Mostly to see the actual z extends +/- from programmed zero is a great benefit when cramming a part on a machine with limited clearance, I do a lot of layered machineing "stack and whack" using the same operations and just changing the depth limits. The graphics on Metacuts is not pretty but its rock solid.

[Thad]

quote:

---

What is the advantage of HST over normal surfacing?

---

I've been away from surface machining for a couple of years now, so I'm not the best one to ask. From what I remember, it outputs smoother machine motion (more arcs instead of 90 degree direction changes) and applies different cutting strategies (uses a different algorithm to calculate the path).

 

 

quote:

---

And, can I use an STL to define the stock?

---

I'm pretty sure you have all the same options as with MC's "regular" toolpaths.

 

Thad

[Chris Rizzo]

I believe your two problems would not exist using the hst.

 

IMHO, and many others, the 3d hst absolutely blow away the old skool toolpaths.

 

1-much, much smoother motion.

 

2-higher feedrates easily obtainable do to very consistent tool engagement. (and smooth motion)

 

3-copy and past ops, no need to reselect geometry.

 

4-select the whole model as drive, use the parameters to control what gets cut. No need to always mess with check/drive all the time.

 

4.1- When everything is selected, mcx "sees" the entire part and all surfaces and areas, eliminates chance of collisons/gouges. (as long as you keep it in feed move, and not rapid, as mentioned previous)

 

5-all toolpaths have the option to be used as a restmill, thus cad file is there too.

 

6- I can program a part in probably 10% (or less!) of the time it takes compared to the old skool toolpaths. Run time is generally much faster too.

 

7-I'm sure there are lots of other advantages I'm forgetting.

 

8- give your self a crash course on the hst at www.streamingteacher.com

 

I'm going out on a limb here, but I'd say two equally skilled competing shops, one using hst and one not, the traditional shop would be out of business shortly.

 

I still use old surface tp when I'm cutting primarily a 2d part and just need to 3d a surface here and there.

[Colin Gilchrist]

Chris pretty much hit the nail on the head. The HST toolpaths are the newer surface roughing and finishing toolpaths in Mastercam.

 

The only dis-advantage is that you will get lots more NC Code. With your controller, that shouldn't be a problem.

 

To expand on what Chris was saying:

 

The HST roughing/finishing toolpaths are designed to smooth out the tool motion, to avoid sharp corners in the toolpath. With these toolpaths it makes it much easier to take advantage of chip-thinning techniques. There are a bunch of threads where these techniques have been discussed.

 

Basically you are taking lighter radial cuts (stepover), but increasing both the feedrate and Length of Cut. This actually gives you a greater volume of metal removal (cubes per minute), and increases your tool life considerably. It is also much better on the machine.

 

The other option with these toolpaths is axial chip-thinning, but you need to invest in "high feed" tools. These tools have specific geometry on the bottom of the tool (flat and corner geometry). These tools allow you to take light axial depths of cut, with incredible feedrates (due to the chip-thinning process), to give you good metal removal, while producing very little stress on the machine. Another advantage of these tools is that the light axial depth cuts give you roughing paths that leave a very consistent amount of material on the surfaces.

[Reko]

Chris/Colin,

 

I guess I didn't realize there was that big a difference between the standard surface toolpaths and HST. I haven't started the final portion of this part yet, so I'm reprogramming it with HST/Restmill.

 

After setting all of the variables and giving it the STL file, it takes off to begin processing, but then nothing seems to be happening. When I look at the Windows Task Manager, it says Mastercam is processing at 50% of resources so it is clearly working, but the normal cues/information at the bottom of the screen aren't there.

 

Because it appears nothing is happening, I went to exit out of Mastercam and there is a message that Mastercam is "multi-threading" would I like to close?

 

I guess my question is, is this normal to HST because it doesn't happen on other surfacing options. I usually have to wait for the processing to end before I can do anything else.

 

Anyway, I'm going to let it run for a while and see if it generates a toolpath.

 

Thanks for everything :>)

 

BTW, Colin, I'm currently using Mitsubishi's High Feed cutters at 80-200 IPM feedrates on other parts. This part, my tool is 30" out of the spindle so I'm having trouble running it faster than 20-40 IPM... but you're right, High Feed cutters are very impressive.

 

Now I just have to figure out HST :>)

[Colin Gilchrist]

Reko,

 

There is a new "Multi-threading" option for the HST toolpaths. When it is running you will see a little icon on the toolpath that looks like a spool of thread.

 

Do this: Go to the "Documentation" folder in your Mastercam installation directory and read the "What's New in Mastercam" PDF file. Click on the "Mill Level 3 Enhancements" section, and the first thing that is described is the new Multi-threading" functionality. It basically allows you to setup a toolpath (enter geometry and parameters), then Mastercam processes this toolpath in the background while you are now free to do other work.

 

Personally I just turn off the "multi-threading" in the Configuration file so it processes like a normal toolpath.

 

One thing that might be hanging you up is doing a "Restmill" toolpath without a containment boundary. I've found that these toolpaths will process much faster and give you a more consistent result if you always use one. Also, what are your filter tolerances set to? How much stock are you leaving with this path? I try and keep my total tolerance at about 10-20% of my stock to leave value. If you are leaving .05 of material, I would recommend a .005 tolerance, using a 2:1 filter ratio.

 

 

Using a larger tolerance dramatically improves processing time. The place where you want to have a tight tolerance is surface finishing.

 

The Mastercam Reference Guide PDF file does a decent job of explaining all the HST toolpaths, and how the settings effect your toolpath. You can launch the Reference Guide right from the Help menu.

 

30" Tool length?

 

HTH,

[Reko]

Colin,

 

Thanks for the info. The Mastercam PDF file on the "Mill Level 3 Enhancements" was a good read. I usually leave the total tolerance at .001 even when roughing so opening that up is a good tip. Thx. I always use 2:1 filter ratio but I haven't used the smoothing yet. I hope it is as good as advertised.

 

I like the multi-threading. I always wondered why I had to let the computer sit while a tool path processed. I guess I'm not sure why you turn your multi-threading off.

 

And, yes, 30" :>) Huge parts here. The one on my machine right now weighs about 30,000 pounds.

 

Thanks again for all of your suggestions :>)

[Colin Gilchrist]

The honest truth is that there have been some folks around here that have had problems with Multi-threading being left on. I'm thinking things are cleared up in MU2, and to be honest I never had a crash that I can be sure was related to having multi-threading turned on.

 

So really, it is just paranoia on my part. The problem is that I've been doing some big programs and I can't afford to have Mastercam crap out on me. Part of the reason Mastercam is rock solid for me is that I don't give it a chance to get glitchy. I save my files often, I run ram-saver constantly, I use NoHist like it is going out of stye, and the paranoid habits continue.

 

The thing to keep in mind with the filter is that the tolerance is bi-directional. So a .005 total tolerance is really like +-.005. So if you have .05 stock to leave, you might have places where the stock is .043 and some where the stock is .055.

 

The Reference Guide (much longer) is actually a pretty good read too. There are lots of tips for getting the most performance out of all the toolpath types.

 

Have you tried the new 2D High Speed toolpaths yet? You really need to check out Dynamic Milling. It is the best pocketing routing Mastercam has ever had.

[Chris Rizzo]

quote:

---

And, yes, 30" :>) Huge parts here. The one on my machine right now weighs about 30,000 pounds.

---

wow send pictures!

 

A part I'm on now literally weighs about 1 oz.

 

multi threading is pretty darn solid. I've had my share of weird issues lately, and it seems mt didn't have anything to do with things. Go under "view" and turn on the multi-thread manager to see what's going on behind the scenes. Turn your task manager on and watch the first core peg at max.

[Reko]

Colin,

 

I haven't tried Dynamic Milling yet, I've been programming surfaces and trying to come up with good ways to remove a lot of stock. I'm done with this part, and on to some plates. Hopefully I'll have a chance to use DM soon.

[Reko]

Rizzo,

 

I just started here about 5 months ago and I've never worked on, or even seen any parts this big in my life. I'd take some pictures and post them but I don't want to get into trouble 'cause I am pretty new here. Go to the top of this thread and check out the picture I put on photobucket. The biggest internal radius is over 5 foot. You could drive a truck on the machine I run.

 

A 1 ounce part, eh? After lugging some of the clamps and blocks around to set up my parts, I'd live for something like that :>)

[GI George]

Reko,

 

Where are you in Michigan?

[Reko]

Mid-Michigan, Tri-City Area :>)

 

You?

[GI George]

Actually I am in the Mid Michigan area too.