Hi Matt, When you checked the "relative to WCS" box did you also enter your offset in the other box? If you don't do this MC will start assigning offsets for you....one for each view. I always go into my view manager and make sure that all my views for a paricular WCS have the same offset assigned.....which is effectively what you ended up doing. To make this easier you might want to think up some labeling structure for your different views. Often my first view is a copy of TOP, so I'll make a copy and label it S1 WCS A0. I then use this to generate my views (rotate view ,etc...) and label them S1 Axxx (better say thanks Colin G. before I get slapped for copyright infringement). Next setup becomes S2. Its easier then to go into the view manager and ensure that all views from each WCS have the same offset..... Cheers Nick

+1 for memory allocation. Our IT guy did it for me and it definitely made a difference. If you are doing a lot of verification your RAM will still get "clogged". RAM saver and reboot sometimes will help. You can also try not verifying the whole program at once. I usually build an .STL library for every 5 - 20 ops depending on part complexity. Use your most recently saved .STL as your next startpoint Having said that I have also had this break down and then had a successful verification doing the whole program......go figure. .STL files are basically loads of triangles as a mesh. As the cutter moves through the material new triangles are created to represent the new surface. So if you mare doing a lot of fine pitch stitching the number of triangles (and therefore file size) skyrockets. It only takes one of the thousands of triangle vertices to not meet perfectly to start generating error messages. You can reduce the number of triangles in the mesh in MC, but it is cumbersome. If you do a lot of .STL work it might be worth investing in software with more .STL functionallity than MC has. Rhino has all kinds of .STL tools - mesh repair, bad triangle mapping etc... Plus you get some good surface tools.... I have several complex parts with similar .STL file sizes (and greater) and I have never had to increase my tolerence to greater than .001/.001....although it has sometimes beeen a battle... Cheers Nick

Hi Steve, These are 30,000 spindles with 4 figure feedrates. What wouldn't even be considered a crash on a 20K machine can be death to the spindle. They really had to tighten up there verification procedures to meet the rerquirements. Also the machines were a relatively new product at the time so there were various bugs in the system that had to be sorted out....I believe Makino helped them out with all this. They are flying now tho'....!! We have Matsuuras with Camplete....as I said before it seems to be a pretty good set up. I've run plenty of Matsuuras and have always liked them. I haven't stepped up to the plate on our 5ax yet....we've also got plenty of 4ax machines to keep going and we have a couple of guys with 5ax experience. Cheers Nick

I think Steve has nailed it. One of the most difficult things to deal with is mangement without sharp end experience. Simply buying a machine and plugging it in doesn't automatically give you profit. Whenever you move up a notch in technology it doesn't become easier it becomes more complicated - the post and simulation software are great examples. Unfortunately some people are on the never ending quest for the one toolpath/tool/machine that is going to solve all their problems.....it has come to my attention that in this game there is rarely if ever a "free lunch" - just pile the material in the general vicinity of the machine and the parts will make themselves!! I always try and talk about real costs in spindle downtime, as losses off the bottom line tend to get the attention of the management. Good luck on your mission!! Steve we have a local company who were the first on the block with Makino Mag4s, when they delivered the first machine they also delivered a pallet of spindle cartridges. They went through several on their learning curve....and they have some very talented and experienced machinists, programmers and managers!! Cheers Nick

Cool you heels 3DMASTER, my comments on experience were addressed to machin-pilot and his response ..... Cheers Nick

mchin-pilot, I can only assume that your experience with a range of machines is limited. I have run everything from Makinos to Fadals and the difference between them is huge. Cheaper machines wear out faster, break more often are less rigid.....I could go on. All this translates into loss of spindle time (and therefore profit) on cheaper machines as you address these issues. Using a ballpark figure of a $2000 loss for every shift a spindle is down it doesn't take long to close the "price gap" between the cheap and more expensive machines. Not to mention the loss of customer relations due to late parts...... Cheers Nick

By simply going from TOP to BOTTOM you have effectivly apparently mirrored you part (actually its not a true mirror its a reversal of axis). Look at your axis direction arrows relative to the part as you change between your two views. You need to edit your view or your blend chain geometry or both depending on what you are trying to achieve. Cheers Nick

The whole point of adding extra axis to a machine is to be able to reduce the number of set ups to make a part. Sounds to me like they are offering a 3 axis machine with a five axis table bolted to it. I would check out the angular travel and how the 4th and 5th axis are integrated into the system. Can you get continous output from all axis simultaneously or only indexed output from some of the axis? The problem with Head-Head machines is that there angular travel is restricted in your two additional axis. They are also less rigid due to all the additional "joints" and all the extra weight high up on the frame(top heavy)and tend to be slow; moving all that mass around so high up. There are some true high speed head - head machines with good angular travel which don't (because of the high speed spindle) require as much rigidity....your probably looking at $600,000 min. for one of these, plus you open up an entirly new can of worms for tool balancing. Trunion type machines have a wider angular range and better rigidity and are generally faster. We have Matsuras here and although we have had a few problems they seem to be be performing well. I think they come in around $350,000 - $400,000 per spindle. Generally you get what you pay for in machines so if you are only paying $150,000 for a 5 axis machine I wouldn't expect a stellar performance. I wouldn't go that cheap on a 3 axis machine if I were buying for my shop.....which I don't it should be said..... Cheers Nick

We had a a Hass which ripped the tool carousel off the mountings because of this problem. We started using a dry lube spray recommended by our techs,the name escapes me at the moment. End of problem. And it helped protect the taper on stored holders. Pull stud torque as mentioned above is also important. Its surprisingly easy to deform the taper on the holder, especially 40 taper Cheers Nick

I think this is due to the fact that Verify is actually a module from a company called Light Waves (you might have noticed .lwn files = light waves native"). Setting up stock in verify sets up the module and I suspect settings in Stock Setup integrates with Mastercam. How it decides where it is going to default to on start up is a complete mystery to me. And every now and again it changes..... Perhaps Colin from Boeing could give us some insight here......if he's awake yet, bankers hours at the big B....!! Cheers Nick

You could use a "right" compensation and force the cutter to the other side of the line with negative stock to leave on walls. Bit of a cheat and dangerous if someone comes across it and doen't understand whats going on. Would need to be flagged somehow..... Nick

Hi Columbo, Go to the Finish Blend Parameters tab . Hit the Tolerances button and you will find the make arcs in planes option - plus other options which combine to give the "up-front" total tolerance on the main tab page. Is the surface derived from an arc or a spline? Converting to an arc derived surface may help. Finally on the same tab hit the Blend button. This will display the frequency that mastercam is looking at the blend chains for positional information. It usually defaults to the stepover. For a simple shape such as a cylinder you should be able to open it up considerably and thus reduce your code. This will not convert to arcs tho'. Cheers Nick

There are i fact two different algorithms out there for calculating cutter comp: 1) "Yasnac" method 2) "Fanuc" method I won't bore you with the details. The only machine I know of which allows you to select which type to use in the control is Hass. There may be others. Do you use Comp. in control? Using Wear comp. might help. You could try running comp. in computer to see if this cures it....this might suggest a fix..... Cheers Nick Eaton

Having glanced through the above thread and posts I think belearner might benefit from a general overview rather than indivdual examples, so here goes. On the whole climb cutting allows you to balance the cutting forces and achieve a more accurate cut. There are exceptions. Removal of an abrasive/hard skin is one. Waterjet can help on some matrials but nothing can be done about the nasty skin on Titanium extrusion and forged block. As mentioned above, with a conventional cut, you are entering virgin clean the material rather than constantly slamming into the nasty skin if you use a conventional cut. Another technique I use frequently is rough conventional cutting vertical walls in aluminium. If you use one of the free cutting 90 degree shoulder insert mills such as Dapra there is nowhere for the chip to go when climb cutting a vertical wall and so the chip gets forced between the wall and the insert. This can cause material smearing and heat the part up from the friction (potential thermal distortion). Conventional cutting scoops the chip out and ejects it away from the wall. With a good free cutting insert you should only notice a 5 - 10% increse in tool pressure. These are "special" circumstances and generally the choice of whether to use a conventional or climb cut is more to do with the dynamics of the chip formation. On a climb cut the thickest part of the chip is made first, as the cutter advances the cutting edge impacts ahead of the direction of feed. The chip then thins out as the cut is completed. On a conventional cut the thinnest part of the chip is formed first,as the cutter advances the cutting edge impacts behind the direction of feed, and the chip thickens through the cut. Climb cutting, because of the initial high force impact followed by a falling off of force as the chip thins will have a tendancy to push the material away from the cutter. Conventional cutting will tend to pull the material towards the cutter as the forces increase through the cut as the chip thickens. A machined free standig wall will therefore tend to thicken towards the top (the flexible section of the wall) if you climb cut or thin out towards the top if you conventional cut. The implications of these dynamics can be divided into two sections. Physical/geometric implications are that a climb cut will have a tendancy to "hook" any corner or cusp and either have an unbalanced load surge or set up unwanted vibrations (chatter) in the system. A good example of this would be trimming the ends of extrusion with a standig wall or leg. There is little or no flexiblity along the length of the part so you don't have to worry about sucking the part in and undercutting, so a good candidate for conventional cutting Cusps can be a real problem in "tough" materials such as Titanium and Inconel for the above reasons. Thermodynamic implications are more important for people in the aerospace machining world because many aeropace materials are "heat resistant", Aluminium, Titanium , Inconel and high chromium content stainless steel(324 - 348)are all heat resistant materials, i.e they do not conduct heat well. When climb cutting the cross sectional area (and therefore the volume)of the chip is at its maximum when the majority of the heat is being generated, at the initial impact and shear. Maximum heat build up is just behind the cutting edge and slightly back on the chip side of the cutting edge. The higher the chip volume at this time the more heat will naturally flow into the chip and not the part, which can lead to distortion. On a conventional cut large amounts of heat are being generated when the chip is thin. Frictional forces (which are converted to heat) are much greater as you push the cutting edge through the material at greater depth and the chip thickness increases. This can be OK in steel or heat conductive materials but can be a real problem in heat resistant materials as the excess heat will bleed into the part, again risking distortion. This problem is magnified with insert cutters which generally have a nose a few thou. in radius (up front sharp free cutting inserts are an exception as mentioned above). So conventional cutting in tough heat resistant materials with inserts is a bit like trying to pierce the material surface with a ball bearing at an angle. The forces and and heat generated are great and the insert will rapidly break down. Conventional cutting with inserts in Ti or Inconel will normally end in tears...... As the above implies conventional cutting is best done with HSS cutters as you can grind the edge sharper than carbide and thus reduce the above effect, you are also going slower so you are generating less heat. Solid carbide is sort of half way between. Much sharper than inserts but not as sharp as HSS. I conventional cut with solid carbide in Al if I am forced down that road and have even done so in Ti. But it is HARD on the cutters especially in tougher/harder materials. So climb if you can and pay attention to detail when conventional cutting, and only do it when you are forced to. A bit long winded but I hope this clarifies. Cheers Nick

We use Harvey Tool....not a full sphere but it will get to most things..... HTH Nick

I think the chatter problems are because of the type/size of cutter. I've never been a fan of 1" solid carbide 3 fluters. Even in a super rigid 50 taper system with lots of HP they just don't seem to cut smoothly. Not to mention the expense..... On a Hardinge 40 taper they are way overkill. You just haven't got enough HP and rigidity to overcome the torque forces at the cutting edge so the whole thing starts vibrating. 5/8 or maybe 3/4 will allow you to achieve maximum material removal rate with this machine at a far lower price. Up front sharp free cutting insert cutters are the other option if you are set on the diameter, Dapra (as mentioned above) and Misubishi are examples. Your maximum material removal rate will be 4x the HP (continuous) of your machine in cubic inches per min.. You can use any radial and axial engagement you want to suit your cutter. You should try and use the highest spindle speed which gives peak HP on the torqe curve of the motor, this will allow you to keep a high chipload (.006+ - I prefer to run .01+) and prevent thermal distotion of the part. As far as programming strategy I like to look at each part/machine system indidually. Somtimes I'll use short axial broad radial engagement sometimes the other way around, this is usually driven by part geometry and the cutter you select. Hope this helps Nick

Forgot about that new oscillating option...Thanks Mike!! You only need about .005 - .02 ramp per foot of material. I have only done this on a mill, but I would imagine the same theory applies on a lathe. If you don't have much straight line ramping distance you will probably be better off just varying your cut depth. Nick

Depth of cut notching can be a problem in difficult to machine heat resistant materials such as Titanium and Inconel. I have used ramping to control notching mainly in Titanium. Inconel is an even "tougher" material than Ti and is more abrasive due to high nickel content and so will resist ramping even more. Inserts are not sharp and have rounded "nose" and ramping is kind of like a conventional cut. The best analogy I have heard is that it is like trying to pierce the surface of the material with a ball bearing at an angle, the cutting edge is always trying to "push off" the surface. This is why you must climb cut with inserts in these materials. I have conventional cut with solid carbide but its usually fairly ugly and I only do it when I am forced. HSS cutter are OK because they are ground sharper. I would set up the job normally and see if depth of cut notching is a problem before doing something about it. There is no Mastercam toolpath that I am aware of that automatically gives you the kind of ramping you need, you really want to ramp up and down so you are moving the cut line back and forth over a range of cut depth. You would have to create geometry to drive the cutter. Don't know about UG. I used to do mine in APT, which was fairly straight forward.....for APT!! The size of your part (larger parts are easier to use ramping), horsepower of the machine (the higher the better), rigidity of the overall system (remember the cutter is trying to "push off" and not take a chip) and the type of cutter (free cutting tools such as 45 degree facemills are preferable) you use will all impact your ability to use ramping to reduce notching....and you will never illiminate it. Not a material for the feint hearted. You can't just stop in a cut as with Al. So do your homework , can't stress this enough....maybe some test cutting if you have never machined Inconel before, and try and find someone who has done something similar with a similar machine/setup to get you in the "ballpark". Your optimal parameter range will probably only be +/- a couple of percent. Good luck Nick

Hi All, Just thought i'd throw my two cents worth in. The best system I have worked with was when I worked in a shoop which did not save "G code" files. When the job was done the file was deleted from the control. Next time the job was run a fresh posting was executed. No problems with duplicate and "junk" files to confuse the issue. The "latest and greatest" prog was always running This requires: 1)Updating source file religiously, especially during prove out. 2)Clean posts. Using (especially heavily editted) "g code" files means that if you want to move to a new machine, say from vertical to horizontal, or if you loose the "G code" file, you are back to square one on set up and prove out. This system worked great. Only one out of 6 or 8 shops I have worked used this. The rest used (somtimes heavily editted) "g code" files......nothing but trouble...... Cheers Nick

Not really an IT guy but I was having some issues and our IT person said that a certain percentage of the processor memory is allocated to the operating system. He reset this value for me which "allowed" Mastercam to use more of the Core memory. It certainly helped on my computer.....don't know if this is the same situation.... Nick Eaton

I think the important thing here is the surface footage rather than the actual type/brand of cutter. Bear in mind that carbide has to reach a certain temperature to cut efficiently. Too low a surface footage is ALMOST as bad as too high a surface footage as far as tool wear is concerned. This is why simply "slowing it down" often leads to nothing but lost profit, Nick Eaton

PaceToolmaker, Generally we start with either a block or a casting. If a block I extrude a quick soild model, and in the case of a casting we will usually get a solid model from the customer. Place the solid(block or model) where you want it in Mastercam, for us this is normally driven by models which come from our tooling dept. As you start to generate toolpaths you can begin with the "select solid" in verify. After running your toolpaths save the result as an .STL file (we have a file system wich allows you to identify which file represents the verification process up to a certain operation number). For the next operation(s) you verify, instead of using the "select solid" function use the "select file" function and start with the previously saved file. Then reepat. Eventually you will have a "library" of files representing the part at different stages of machining. In the STOCK set up page chose the DISPLAY FILE option and tick the Display and Solid check boxes below. Select the file you want to display via the button at far right of the file dialouge box and your .STL will be displayed as a translucent solid over your part (which you have in position within your material envelope). You want to use contrasting colors between your solid model and .STL so that areas of the .STL which drop below the model surface (gouges) will show up. I generally use 86 for the model and 177 for the .STL (set in config. file) so gouges show up as bright green spots in a sea of dull red. "Tigerstriping" inidcates you are right on the surface. As you move from one set up to the next you will either have to translate your last .STL from the last setup to the new setup position or constuct a new WCS for your subsequent operations. As mentioned above translating the .STL is not as contollable as translating entities but as you use this method you will begin to figure out ways to make it a little quicker. I generally use this metod as most of my programming is 4 axis includig a fair maont of "live" 4 axis stuff so I like to keep my WCS on Mastercam Zero. Always make sure you are in TOP in the STOCK file page or your .STL will start moving around the screen. I work in an Aerospace job shop, so these methods might not suit you but hopefully you can get an idea of the functionality and modify to suit your purposes. Cheers Nick Eaton

It is possible to set up a VPN site to access license from home. You need a good IT person to get it to work well and there are scurity issues.

I would rough the part first with a minimum rad tool (.02-.03). Ballnose endmills are not very efficient chip makers and you really want a uniform chip with as high a chip load as possible (.006 or higher) to keep the heat in the chip and avoid distortion. I am roughing 18" long slots in our Kitamura 20k with plus head at 19000 and 650 ipm with a .17 cut depth with a 3 flute .375 cutter. Ultimately your feedrate and depth of cut will depend on your horsepower and system rigidity. To get proper speeds and feeds for ballnose finishing you will need to calculate effective surface footage and chipload. Again keeping the effective chipload at .003-.004 will save time and avoid distortion. You will have to make several calculations as the effective surface footage and chip load will change as you work around the radius. As an example with .5 inch 2 flute ball,.02 depth of cut and .01 step over 18000 rpm and 650-700 ipm on a 45degree angle gets you in the ball park. Twice as much feed on the flat (bottom of your channel). Keep an eye on your load meter when roughing. If you are not running a 70% load you can probably go faster or deeper. Hope this gets you started Nick

Try looking in your system configuration/Cad Settings page. Have you got the Reset Cplanes to Top in Iso Gview Selected? If so unselect it Hope this helps Nick