Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Cnc programming
- Thread starter vikes1
- Start date
- Replies 35
- Views 3,733
theperfessor
Cast Iron
- Joined
- Sep 15, 2011
- Location
- Southern Indiana USA
Depends on a lot of things. What feature is the dimension applied to?
Everywhere I've worked we would program to 0.995. The idea was that 1.000 +0, -.01 is pretty much the same as 0.995 +/- .005 (I know, I know.. it's not but effectively it is). You have more chance of getting more good parts off the machine if you (correctly, IMO) assume you can equally likely be over as under on any given dimension.
johneezreno
Aluminum
- Joined
- May 31, 2018
Same boat. Cut tolerance in half and go that route. .995
Sent from my SM-G950U using Tapatalk
Sent from my SM-G950U using Tapatalk
mhajicek
Diamond
- Joined
- May 11, 2017
- Location
- Maple Grove, MN, USA
If you have a plus tolerance feature and a minus tolerance feature both programmed at nominal and cut with the same tool, how's the operator going it comp it in?
It is exactly the same. The print specifies the acceptable range of tolerance for a good part, and inspection is binary; the part is either good or it isn't. If the customer wants a tighter tolerance zone they should ask for it and the quote will be correspondingly higher. Likewise it should be modeled at .9950, because doing otherwise can result in impossible geometry.
It is exactly the same. The print specifies the acceptable range of tolerance for a good part, and inspection is binary; the part is either good or it isn't. If the customer wants a tighter tolerance zone they should ask for it and the quote will be correspondingly higher. Likewise it should be modeled at .9950, because doing otherwise can result in impossible geometry.
Hardplates
Stainless
- Joined
- May 8, 2019
- Location
- What once was a free country
Something that loose I will program in the middle and let it rip. If its something fussy I will often program on size and comp the tool and rerun till I sneak up on it.
13engines
Stainless
- Joined
- Jun 30, 2015
- Location
- Saint Paul, MN
I tend to agree with the comments about shooting for half allowance and go from there, then working your way as close to nominal as you dare, but in a CAD/CAM environment, you would never start reworking CAD drawings so that the lines in the drawing are different then nominal as I'm sure they're drawn originally. What a nightmare that would be. The tool path coordinates are generated directly off the drawing, so nominal is what you're working with. If you're creating and using an offset tool path, sure, include the extra five thou in your settings. But as I've said before, I think all finish passes should be done with comp. I would program to the nominal feature line(s) and be prepared right from the start to skinny up my comps on periphery work and just the opposite on bores. That is, in this minus only tolerance example.
Hardplates
Stainless
- Joined
- May 8, 2019
- Location
- What once was a free country
Although not very fancy simply programing the tool oversize will easily put you in the middle of tolerance without modifying any drawings. Or stock to leave or whatever other fancy feature your CAM program has.
Hardplates
Stainless
- Joined
- May 8, 2019
- Location
- What once was a free country
Whats with you and chainsaws today? Did you buy a new one that you would like to tell me about?
ChipSplitter
Titanium
- Joined
- May 23, 2019
- Location
- Maybe
If you haven't got that figured out I wonder what you're programming.
Smells trollish to me.
The reason I ask is my programmer always does the print dimension and a lot of times the first part is bad. And I tell him to program it to the nominal dimension so your not on the edge of making a scrap part. So I wanted to see if it was standard practice to program to nominal. And yes I am an inspector 
13engines
Stainless
- Joined
- Jun 30, 2015
- Location
- Saint Paul, MN
Yes that's part of what I said. I forget that many CAM programs use "stock to leave" or give you the ability to fudge tool sizes to meet the same end. When I use offset paths in my ancient CAD/CAM software, which I mainly do during roughing, it's more manually derived, where I'm setting tool radius plus the fudge factor into a single entry "offset path" window. I realize now the OP probably never had in mind the idea of altering the drawing. He's likely just asking if he should fudge some settings in a CAM window. Duh. Though using cutter comp at the machine, whether tethered to an offset path or original part outline, is still the best way to control final feature size. My slant anyway.
EDIT: Well hello Mr. Inspector. Perhaps email your programmer a link to your thread here. Maybe he or she will garner some insight form something said by fellow members. Then again maybe not.
tonymor
Aluminum
- Joined
- Feb 9, 2017
- Location
- Chambersburg PA USA
I used to work with a guy who ran a lathe and he wouldn't do either. He'd round his numbers and then comp the tools to make up for all of it. He seemed to be able to keep his comps in his head and get it right again when setting up the next part. No problems there until i had to come in on second shift and try to figure it out. Then i would redo the programs to the nominal and set all tools correctly. Which he didn't like. It took a little while for us to understand each other but we got there in the end.
Simply programming to the nominal probably won't stop your guy making bad parts... There's a little more to it than that.
Bobw
Diamond
- Joined
- Feb 8, 2005
- Location
- Hatch, NM Chile capital of the WORLD
Your programmer is a fricken retard. Who the hell programs to the absolute min or max of the tolerance? A fricken retard... Thats who.
I very rarely run comp. There is seldom a need unless its really tight. For .010 total, if I was actually trying to nail it nuts, I would program external at .994 and internal at .996, unless the tool was stupid long and floppy. The FIRST part would be within a thou of the middle of the tolerance, and I'd be happy. And its in tolerance and I'd get paid.
Your programmer is an idiot. And you can tell him I said that. He's an idiot.
D.D.Machine
Stainless
- Joined
- Dec 10, 2003
- Location
- poulsbo, wa, usa
I am with mike on this one ,, I program to the middle of tolerance, so I would program to .995 and use that as the base to set my +/- when I was checking the part , it gets to screwed up if some dimensions are plus and other dimensions are mines ..
Glad you came on here and asked ,, we learn as a community by helping each other out
DMF_TomB
Diamond
- Joined
- Dec 13, 2008
- Location
- Rochester, NY, USA
.
depends on many things. often a M0 is added at tool change with a warning or message like adjust comp tool and take test cut, assumption being after test cut measure, adjust tool comp and rerun and find it measures very close to target
.
sometimes find test cut shows a problem due to tool taper wear for example or corners broke off
.
yes most operators find its easier if programmed toward center of tolerance cause if tolerance wide enough often you dont need a test cut or recutting. like if you needed to recut 100 out of last 100 parts and if program changed and you dont ever need to recut cause its in tolerance why wouldnt you make things easier ?
.
worse is if something cut too much as programmed and part is scrap and operator can do nothing cause way it was programmed, if no M0 and overcut damage is already done by the time operator measures. safer to cut less, measure and recut than to scrap part usually. many a new program a operator looks at program and adds many M0 for potential problems to not make scrap parts. not everybody does that
G
Guest
Guest
If you haven't got that figured out I wonder what you're programming.
Smells trollish to me.
I disagree on the troll part. I always wondered why an engineer would dimension something at 1.000 +.000/-.010 instead of .995 +/-.005. I have always gotten the same answer,they want the part as close to 1.000 as possible without going over.
