Toleranced features on a solid model

[LancoUSA]

Our engineers here draw every thing on size for holes or toleranced features. Is there a way for them or myself the MasterCam programmer to machine these holes with out using multiple diamter offsets for the tool? I am looking for a way for Master cam to recognize tolerances. Unfortunately we use Solidedge, not Solidworks. Does any one have any ideas? I am new to mastercam this year, and have never gotten too deep into any other cam packages that I have used in the past.

 

Thanks.

[K2csq7]

I am looking for a way for Master cam to recognize tolerances.

Don't think that's possible

[YoDoug®]

I always adjust my stock to leave in Mastercam tool paths to cut to my desired result, usually the middle of the tolerance range. For example; in the solid has a hole that is 1.0 and the print tolerances it at 1.000 +.005/-0 I will set the stock to leave at -.0012 (.0024 diameter). That way assuming the tool is to size and cuts correctly it will cut to the middle of the tolerance.

[BenK]

I always adjust my stock to leave in Mastercam tool paths to cut to my desired result, usually the middle of the tolerance range. For example; in the solid has a hole that is 1.0 and the print tolerances it at 1.000 +.005/-0 I will set the stock to leave at -.0012 (.0024 diameter). That way assuming the tool is to size and cuts correctly it will cut to the middle of the tolerance.

 

+1

 

I also do this for any plating or paint.

[LancoUSA]

I was just checking to see if any one has tried going the route that I would like to see things done. I think if engineering would draw what the finish product should look like and also factor in for paint, coatings or what ever else they want done to it. Then I would be able to machine with the same d offset and material left with out ever having to do much else, drawing extra geometry or what have you. Just an idea right now...

[AshM]

..... Then I would be able to machine with the same d offset and material left with out ever having to do much else, drawing extra geometry or what have you. Just an idea right now...

 

It seems to me that you are looking to exclude your expertise from the production of the parts.... not to be rude, but the guys and gals programming and running the machine tools are the people who imprint their intelect into the parts by actually making them. Its often easier to dream up a design than it is to make it.

 

there are some good ways to deal with these problems, but you always need to do it yourself. Most parts I produce/program need to have selected surfaces or areas produced differently to the print or the model to allow for grinding, hard machining or to get to a tolerance. As suggested above i never alter my Dia. offsets or values, as i aways want my tool in mcam to represent the actual tool in the machine. You need to create geometry to get around this especially if you are going to chain geo for one finish pass where different surfaces/edges within the chain require different stock left or removed for whatever reason.... sad truth. My suggestions are to either individually chain a surface or egde in order set up stock to leave parameters for your result if you don't want to create geo (but this will make you toolpaths inefficient if you are making more than a handful of parts) or otherwise don't be scared to use the control compensation options to hit sizes. If you aim to cut to the centre of the tol (as suggested) and use control compensation you basically cant go wrong if you accuratly set your tool R para in the control...

[LancoUSA]

We are making on off parts all day long. there is rearely any production here. If there is production it is less than 20 parts. that is why i would like the hole at the meadian value. The only problem with using only one d offset is that if i have a +,+ feature, and a -,- feature, and the operator wants to adjust one or the other by a little bit, say it is deeper and may have some spring. It's easier to have multiple d offsets so they can adjust them individually.

[LancoUSA]

the guys and gals programming and running the machine tools are the people who imprint their intelect into the parts by actually making them. Its often easier to dream up a design than it is to make it.

 

 

ASHM,

[LancoUSA]

I agree with you 100% about the designing and machining of parts. I am just trying to come up with a fast way for us to machine parts. Also being able to program them fast. I think my next step may be to look at importing and exporting tool paths for particular size holes. If I can get engineering to standardize on slip fit or press fit sizes.

[AshM]

i'm in the same possition as you are, in that i make 1 or two parts, then the run is over. try using really small finish cuts (on the walls and floors) like 0.15 - 0.2mm and always use a spring pass. that way when the cutter runs the spring pass it is basically just skimming back over the wall you have already cut. you will avoid having to guess the amount of spring in the cutter, especially if the wall is tall.

 

this used to be the thing that people swore was wrong, because it would rub the cutting egdes and blunten the tool, but with carbide endmills i think this is a myth.

 

when you are making only very small runs of parts you very rarely get to use tools to their full extent because the parts and cuts change all the time, and i tend to throw out cutters because they have cut 40 or so 10mm high walls, then the next part needs a 20mm wall (or whatever) but the cutter has worn to show a shadow of the 10mm cut that preceeded.

 

in my experience when you are only making a small number of parts you need to be able to program and setup quickly otherwise you won't ever make any money, so if your program runs for 5 mins longer, but you save an hour programming who cares about some air cuts or some spring passes if the parts come out to size with less stuffing around...

[BenK]

because it would rub the cutting egdes and blunten the tool, but with carbide endmills i think this is a myth

 

It all depends on the material you are cutting. If you cut aluminum all day then you can get away with this, If you cut any steel you should avoid spring passes. To be perfectly honest I can set my stock to leave correctly in less time than it would take the machine to make that cut.

[AshM]

Didn't take long to get some controversy,

 

I am a fan of the spring pass for steel, but I wouldn't do it in a production run. What I'm suggesting is that when you are doing one offs or very small runs most of the time it is rare that tools tend to get "used" to the limit because it will exposed to various materials and grades or conditions virtually every other minute. When you need to be able to program a new part or process in minutes and get onto the next job ASAP programming spring passes and using cutter comp in control can fairly guarantee you will hit your size, and any difference will be in the wear on the tool and that is easily corrected. Plus after a spring pass if you need to make another cut of a small amount you won't need to worry that your cutter will over cut and ruin the job.

 

IMO these benefits outweigh the cost of replacing tools probably only a handful of parts sooner, in a jobbing shop. Efficiency is measurable in "jobs per day" just as easily as "parts per tool"

 

Rant rant rant! He he

[BenK]

As suggested above i never alter my Dia. offsets or values,

or

programming spring passes and using cutter comp in control can fairly guarantee you will hit your size

 

? Only one of these statements can be true.

 

 

I come from a short run background, I know what it takes to get parts done fast. I was offering a suggestion about a fast way to adjust for the tolerance of a hole. If the hole is drawn at 1.00 but the tolerance is 1.00 +.01-.0 just changing your stock to leave solves your issue in seconds.

 

 

this used to be the thing that people swore was wrong, because it would rub the cutting egdes and blunten the tool, but with carbide endmills i think this is a myth.

 

If you think this is a myth than why wouldn't you do it in a production run?

 

Rubbing the tool like that comes down to chip load, you need to have a sufficient chip size to carry the heat away. If your not creating a chip there is only two other places the heat can go, one is the part(really bad if your working with an easily work hardened steel) the other is the tool.

[AshM]

ok here goes:

 

Re dia offsets I never use multiple D offsets for the same tool, so I would never call tool 5 using d offset 9 for instance, only T5 D5.

 

Re spring passes and control compensatation for sizing and tollerances - read above....

 

Wheres the contradiction????

 

Spring passes.... tell me, if you take one pass/cut along an edge, then retake the same cut, does the second pass remove material? the answer is most often yes. A spring pass does actually cut, just very lightly, and might i say, without very much deflection. Thats why its called a "spring" pass, to account for spring... Nobody would do it in a large run of parts because it takes extra time.... but thats not our concern in this discussion is it? we are talking about ways to reliably produce one off or two off parts without having to create lots of geo. to account for differenct requirements on alternative surfaces of a part model to match tollerances.

 

My suggestions arn't for everyone, and quite clearly not you. Historically machinists advocate that using a recut strategy to size parts damages tools is correct if you are using HSS or even high cobalt ones. Using those tools and taking lots of very lights did blunten them considerably and quickly, however now that carbide endmills are readily available and capable, and coatings are so effective this isn't really the case any longer.

 

Any cut or contact between the job and the tool causes wear, but its proportional to load. High load = high wear, low load = lower wear, seems simple enought to me.

 

I think if you give the strategy a go you will find it is reliable.

[BenK]

High load = high wear, low load = lower wear, seems simple enought to me.

 

 

Have you ever had a tool wear too quickly because you were not pushing it hard enough?

[AshM]

Have you ever had a tool wear too quickly because you were not pushing it hard enough?

 

absolutely of course i have. Buts its not a given that this will always be the case. Regardless of the DOC alone effective machining needs to balance feeds, speeds, rigidity, etc also, and when applied correctly a recut method is very effective.

[BenK]

Any cut or contact between the job and the tool causes wear, but its proportional to load. High load = high wear, low load = lower wear, seems simple enought to me.

 

If you have had a tool wear because you were not pushing it hard enough than your statement above is already false. Like I have said before I come from a short run background I know what it takes. I'm not going to sit here and argue with you about this. If you want to burn up endmills then go ahead.