|
|
|
| Home » Knowledge Base » Knowledge Base Article | Login | Become a Member | What's New | Site Map |
|
WOODWEB DISCLAIMS any and all RESPONSIBILITY and LIABILITY for the accuracy and application of the information below. Readers agree to evaluate the significance and limitations of the information provided, and accept full responsibility for the application of this information. Read More ... |
|
|
Would you like to add information to this article? Interested in writing or submitting an article? Have a question about this article? Routing Deeper than a Tool's Allowed "Usable Length" 
Question
Forum Responses
From contributor L: You may be able to change the tool holder as well, or create a new tool and/or holder. What software are you using? From contributor W: What kind of machine are you using and what software? I know on the Biesse Rover that I program, the machine only cares about how long the tool is, and in Mastercam it also allows you to go beyond the length of cut. More info please. From the original questioner: It's a Morbidelli. I'm just writing G-code at the machine in Xylog. Creating a new fictional tool does seem a little safer than altering the normal tool parameters. From contributor T: In some controls which specify tool names for specific tools, there are additional fields called cut length, tool thickness, or thickness. This field is in addition to the length of the tool with the intended purpose of never allowing the tool to be engaged deeper than the flutes. Often when someone needs an application such as progressive deep pocketing, they either lie to the field to allow the machine to go deeper or duplicate the tool in the tooling table with a false thickness value and alternate name for a one shot use. If you are confident that you can safely machine the features, then by all means try this. Be very careful, especially as you achieve your programmed depth - single stepping the program first while cutting air is always the safest option. From contributor J: That's correct that Rover (NC1000) doesn't consider the cutting length, so your Morbidelli may not either. From contributor W: The funny thing is the tool parameters setup on the Rover asks for the tool thickness (flute length), but even if it's set at 1", you can still write a program for that tool to go deeper, and it will. From the original questioner: Thanks for the replies. I'm good with it. I imagine the 5 axis guys run into this type of situation all the time. Is there CAM software that understands that material has been removed and it's safe to go in? Just curious. From contributor J: "The Rover asks for the tool thickness." I think that only applies to boring bits. Being in the same table allows it to be set for router bits, too. If the table was properly designed, it would not allow a tool thickness entry for router bits because each tool has a field for tool type. From contributor K: Sometimes you can't see the forest for the trees. Can you just change the thickness of the wood being machined? I do it all the time on my Ecomaster - change from 1.5" thick to .75" to .5", etc. The machine just has to know how deep to go from the top of the material. From contributor S: "Sometimes you can't see the forest for the trees," and sometimes you run into them. By changing the material thickness, you have to run the program several times and change the material thickness each time because "You're going to be "pocketing" progressively deeper." By configuring the tool correctly, you can write a looping subprogram that includes a Z incremental movement. I suppose you could get cute and change the material thickness from inside the code, but that's not proper coding. You wouldn't change the material thickness to bore a deeper hole. From contributor A: Yes, there is cam software that does the job. We just draw layers of cuts over each other and push the start button. Same as doing it manually by editing the code, except 465,000 times faster. I think you would find that with the new cam software and machine available today, this job isn't a problem. From contributor M: I don't know of any CAM application that could pull tool parameters from SCM point to point or router and change usable tool length on the fly. The simplest way to work around this problem is as someone else suggested - to modify tool settings. I would not necessarily call this lying to your machine since you are using usable tool length as you go around and pocket entities. I would *never* ever change wood thickness to achieve what you want because you *will* crash your tool in to the panel as the machine approaches the panel. As machine approaches programmed panel height, it does that with G0, full speed ahead (at least 45 m/m), hence your tool will break. Not only that, but every time it repositions, it will cut through the panel face. From contributor J: "I can't understand "lie to the machine," "change your usable cut length," and things like that." What part don't you understand? According to him, his machine's software wouldn't allow him to cut any deeper than the tool's cutting length. From the original questioner: Great advice, contributor M. That is critical. I was just watching that this morning while I was using the machine. The G0 (rapid) moves were fast and had the bit just above the board. Thanks again, guys, for the fictional tool advice. I used it and then deleted it. From contributor T: Actually, custom written macros can pull certain information on the fly when needed. Unfortunately, most people do not want to invest in this method of programming because it is not cam written. Fanuc controls are great at doing things of this nature with tool lengths, diameters, offsets and a whole lot more. With the proprietary European based controls it is more difficult and in some cases impossible. Also, just for clarity, the tool length and tool thickness or flute length in this case, are two entirely different fields. I am glad you got the result you wanted!
From contributor M: I need to clarify a couple of things. I said “I don't know of any CAM application that could pull tool parameters from SCM point to point or router and change usable tool length on the fly." Change being the key word. I have used tool parameters in my macros extensively but only as variables in my programs. See CNC Code. The response was for the poster before me who said "Yes, there is cam software that does the job." CAM program does not change tool parameters on any machine as far as I know. But I may be wrong. It wouldn't be the first time. Have you reviewed the related Knowledge Base areas below? 
|
