Accuracy

[brian]

I know this has been dicussed many times.I did a search on this subject and read through the results.I'd still like to hear it directly from those in the know.
I drew up a retangle 2.125 x 11.9375 and ther actual cut came out at 2.117 x 11.9368. I cut two of the same parts and they where the same dia.Is there anyway I can adjust the variables to correct this or do I just adj. my initial drawing.

Thanks Brian

[steve4460]

What version of the sortware are you running ?.
I am having the same problem with 3.27. I went back to 3.26 but haven't had a chance to test it , but I do remember that this started after I upgraded to 3.27
I will run some test tomorrow .

[fleinbach]

The latest software out is version 3.4.30 and I recall reading somewhere, one of the versions between .27 and .29 had some problems. But I do not believe this is a software issue.

Brian,


You did not mention what material you where cutting. Nor did you mention your depth of cut and speed or what size bit you are using and how many flutes. Were you running conventional or climb cut? Was the bit new and sharp?

All of these factors are necessary to form a conclusion to solve this problem.


Your discrepancy is .008 in one direction and .0007 in the other. To be able to cut within 7 10,000th I believe a milling machine would be more appropriate.

[brian]

I'm cutting .75 MDF,cutting .2 per pass at 3in/sec with a .25 up spiral bit which is almost new.I used conventional cut.
Sorry ,I had a typo on my first post.It was of by .007 in both directions.

Thanks Brian

[richards]

Brian,

I often cut pockets that are 1.125 inches in diameter. Depending on the cutter that I'm using, I sometimes have to specify the diameter as 1.1 to 1.135 to get the pocket that I want. Sometimes the difference is a direct ratio of the true diameter of the cutter that I used to the diameter specified to make the cut. Other times, it seems to be more of the cutting characteristics of the cutter, the material, the speeds, etc. than of the expected diameter or cutter diameter. I've learned to leave extra material when cutting critical parts and then do a finish pass after measuring the exact size of the roughed-out part. Without a lot of extra effort, I can hold tolerances to 0.0015 inches. Even with my vertical mill, which is designed to handle heavy cuts in metal, I 'sneak up' on the final size so that I can make a finish pass at 0.020 inch. (By the way, unless absolutely necessary, I always use a cutter that is at least 3/8-inch in diameter to reduce the possibility of cutter 'flex'.)

[harryball]

Just let me ramble a minute...

I'm still not clear on how much error you have... the original post is .0007" on the smallest error and you later stated the error is .007" on both.

Assuming an error of +/- .007" that's less than 1/64" total possible error between cuts. Ending up with the full error is a statistics exercise. I don't know what you are cutting but I'd have to agree with Frank, a milling machine may be more suited to your needs.

You also state that the error is consistent. i.e. you always cut with the same amount of error. Check to see if the error is scalar or static. If you run the small rectangle and the error is .007" then you run a larger rectangle and the error is the same you then know the error is not caused by wrong step counts. i.e. your error does not add up.

If it is the case the error is static check your bit diameter. Since I purchased some undersized Freud bits I'm in the habit of measuring my bits when I'm concerned about tight clearances. I found the Onsrud bits I received to be every so slightly oversized... and I mean SLIGHT. My 1/4" bit measured .25005" whereas my Freud 1/4" bit measured .24920 which was enough to create a DADO fitment problem on one of my kits.

Suggestions:
Check your bit diameter.
Check your error when cutting conventional vs. climb.
Try different bits.
Check your Z axis for square to the table.
Check and tighten all your bolts.
Check your table surface to make sure it is not moving and your clamp down method is secure.

If all that checks out and your error is that consistent, you might consider including a small offset when creating your toolpaths to compensate.

I have to say if you are seeing .0007" in error you have nothing to complain about. It if is .007" that's still a pretty small error but I could see where you might want to tweak it if possible.

Robert

[Brady Watson]

What program are you generating the toolpath with and what do you have set as your toolpathing tolerance in that program?

-B

[brian]

Robert
The .0007 was a error on my part,it was .007.The parts with this error were the same.I made three of them to see if the error was the same,and it was.
The bit is from american carbide and is .251. and is .5 inch shank.
The table suface was screwed down.
I will try the other things you suggested today.
Whats the best way to square the Z axis.I've used a machinist square on the spindle.
I know that .007 is still accurate but wanted to know if this can be improved upon.

Brady
I'm using Artcam pro 8.1 and the tolerences are set at .001.
By the way I read through some of your suggestions on stuttering(which I had a case of)and used task manager to gage my PC's resorces.Got rid of some unwanted programs and the stuttering seems to have gone away.I'm running a 1ghz,256 ram in the shop and any speeds over 7ips tax the machine to its capacity.Thats if I run only one axis.Two axis is even more demanding.
Would more ram solve this problem or do I need a faster CPU.
I also noticed(through Task Manager)that when shutting down artcam that artcam.exe uses up all of computer for at least 60 seconds.Can this also be solved by more ram.


Thanks Brian

[brian]

Just checked my software and I am only using 3.1
What improvements were made in version 3.26 over 3.1.Is it worth the time to upgrade.

[Brady Watson]

Brian,
Sounds like you have a few issues going on. 1st, your CPU should be at least 1GHz and I would recommend at least 512M of RAM. XP eats up more RAM than previous OS and there is no such thing as too much RAM.

ArtCAM should *not* be installed on a computer that is running a tool. Whether or not the dongle is in there or not, the program still looks for the dongle behind the scenes, EVEN when the program is not open or running. This has been known to be a source of disconnects and comm errors. Even PW can cause problems when it is left minimized while running a tool.

You say you are running 3.1...by all means upgrade it to at least 3.4.26 as there are numerous improvements. You will (should) see an increase in smoothness and communication in the later versions of the software.

-B

[brian]

Brady thanks for the quick reply.
I installed artcam as it was convinent to use as my designing computer is a good walk away.I will be adding on my shop soon as this is only really a hobby at the moment.It wil save me from moving my dongle around.Then I can squeeze my other computer in my shop.
I want to spent some time learning before hanging out my shingle.
I will delete artcam today!
More "ram" ya say.Hey have you noticed how male that sounds(Ram,Dongle) :-)
Thanks for the info
Brian

[Brady Watson]

Brian,
I do most of my work in the office/studio in Pro and then export an EPS of my vectors along with the SBPs across the network to the shop. I have PW2 installed in the shop & if I have to re-toolpath something, it saves me a trip. Most of the time I am cutting a 2D part...3D parts I still have to run inside to change.

-B

[harryball]

Brian,
.007" is pretty good... but probably tweakable.

Setting the Z square is a big deal to some folks. I square my Z using the Zeroing routine... http://www.talkshopbot.com/forum/messages/7/15082.html?1158926563
Technically the Z out of square wouldn't cause your parts to be the wrong size just rhomboids from the side. It does, however, effect the measurement depending on how you measure the part since the sides would have slope to them.

Gantry flex is another issue, one way to "see" the flex is to cut conventional vs. climb and note the differences. Bits can also flex, but the 1/2" shank should reduce that. I don't know how to reduce gantry flex, it's not really been an issue to me so I've had no cause to consider it a problem.

Robert

[brian]

Brady
One day I'll be able to hook my computers together.I don't have the internet in my shop,I'm trying to keep things simple at the moment.I have PW2 but I figured artcam would be a better program to run.I'll reinstall PW2.
Robert
I have an alpha and I assumed they had solved most of those problem in the newer model.As you can see in from above that I'm not pushing it enough to cause gantry flex.

Thanks guys
Brian

[richards]

Brian,
Try this experiment. Cut two identical rectangles with the 0.25-inch cutter at 0.20 depth, 3-ips, just like your post above. However, cut one rectangle with a climb cut and cut the other rectangle with a conventional cut. You may be surprised at the difference in size. The rotation of the cutter pulls the cutter into the cut when going one way and pushes it out of the cut when going the other way. To me, it's like a needle following a groove in an old vinyl record; even though there is significant mass in the arm and in the turn-table, the needle is the part that vibrates. The same basic thing happens with my 60x120 Alpha. Lots of mass in the steel table. Good sturdy X/Y/Z axes. But, it all depends on a little, flexible 1/4-inch cutter that is being spun at a tremendous speed and forced into a cut by a mass probably well over 10,000X its own puny mass. Something has to flex.

If you have a dial indicator handy, turn your machine off, zero the dial indicator with the dial perpendicular to the cutter and then give a few pounds pressure to the side of the cutter opposite the dial indicator. I'm guessing that you'll see a lot more than 0.007 inches deflection.

[harryball]

I'm running a new Alpha as well, there is gantry flex, bit flex and so on, try Mike's test, you might be surprised.

Robert