Ideas? (new Dad/Son team) CAM to part is .002 to .005 over. Things 2 check?

The Son (newly minted graduate)is giving it a go in job-shopping. The short of this is,
stainless 316 part. Done in Solidworks w/ HSMWorks CAM.
Ran first 2 operations.... X is .005 too wide. Y is .0025 too wide. Running a 98 Haas VF/4 we rebuilt.

He USed a lot of HSM CAM features. Adaptive clearing, Tooling radius is set via CAM gCode, Stock settings etc. He has checked and rechecked all his work. Measured w/ 2 different setups. it's off.

He's done ALu-6061 before and our smaller test blocks are all spot on. He thinks its the machine and I think it's all the elaborate CAM.

While this could be any number of things... I get that. Wondered what some of the Brass here might think as a top one or two things to check/try...

He is going to recut his ALU part again tomorrow as a test.

Did you run skim passes....

countryguy said:

The Son (newly minted graduate)is giving it a go in job-shopping. The short of this is,
stainless 316 part. Done in Solidworks w/ HSMWorks CAM.
Ran first 2 operations.... X is .005 too wide. Y is .0025 too wide. Running a 98 Haas VF/4 we rebuilt.

He USed a lot of HSM CAM features. Adaptive clearing, Tooling radius is set via CAM gCode, Stock settings etc. He has checked and rechecked all his work. Measured w/ 2 different setups. it's off.

He's done ALu-6061 before and our smaller test blocks are all spot on. He thinks its the machine and I think it's all the elaborate CAM.

While this could be any number of things... I get that. Wondered what some of the Brass here might think as a top one or two things to check/try...

He is going to recut his ALU part again tomorrow as a test.

Click to expand...

If he's trying to cut right to finish size with an adaptive path...yeah, not gonna work. Need a different toolpath in for finishing.

Agree with dodgin (if that is what you are doing). HSM paths are great for roughing, but you need a separate toolpath for finishing. A simple contour (in mastercam), or a profile or whatever solidworks calls it... Also, make sure you have a lead in/lead out move to turn comp on and off (most machines want/need a straight line move for comp to activate...)

What does the finish path of the code read? That would tell you if its the program or the machine. I'm gonna lean towards cutter comp and tool deflection if you have your axis thrust set right and after the rebuild you set the machine comps correctly.

When you rebuilt it did you renew the ballscrews? The heavier tool pressure cutting stainless may be pushing it in the backlash. Also as the above posters mentioned, the final toolpath may be the culprit.

Ed.

Hand code a square milling all four sides to ensure the machine is milling to size

try running the program twice on the same part and see if the dimensions change[they will to some degree]

I know some CAM programs have a stock left box, and it may have a non zero default number if you don't override it

In my opinion nothing is “perfect”. Take a spring pass. If that doesn’t fix it then put -.002 in the “stock to leave” box in HSMWorks. No big deal in my opinion. It could be your setup, your speeds/feeds, tool deflection, etc. You will get to know the machine better and account for it automatically depending on the job. I don’t see anything unusual. Lots of times I have values in the Stock to Leave box. I would setup one profile to intentionally leave .005. Then measure and if it actually left .007 or .003, then the finish pass you know what numbers to use based on the real measured value. I do this rather than a spring pass or second finish pass in anything other than aluminum. You need to be cutting something or your rubbing.

Could also be a worn out spindle taper. Check that as well.

But on second thought if you continue to get different numbers for x and y you might need to investigate that. But on the other hand, solving one axis with better toolpaths and offsets might fix both

Aluminum and SS being different materials need to be treated differently in both roughing and finishing.

What also needs to be understood is that CAM is just a tool, like all tools you need to learn how to use it. Just because the display can render the part correctly and spit out code does not mean the part will come out correctly.

If the machine is a bit out...as a machinist you need to take that into account and compensate for it.


I think what it boils down to is experience, you cannot blame the machine or the CAM for bad parts.

You mentioned oversize in SS.

A finish pass in 316 can have a tough surface that was left a bit over by a roughing pass...so your tool can spring in more on a finish pass.

A roughing op in tough material can have tool deflecting, work pushing giving you off centered features...now when you clean up, if off center enough you wind up overcutting.


So the question is did the part get measured prior to the finish cut? Do you know where the problem came in? Need to know that to figure out how to correct. You may need to leave a bit extra on your roughing for a spring pass prior to the finishing pass.

You say "rebuilt". To so e people that means painted. Please elaborate.

I would program a very basic square with your CAM using 2d tool paths. Read the code and see if it is posting what is expected. If so, I would run the part and see what your results are. If its different than what is programmed you have a machine, tooling, fixture or setup issue.
If he is "profiling" a contour using a ballnose tool or a tool with a corner rad I would check the tolerance of the radius on the tool. Some tools are pretty liberal with the tolerance they hold the tool nose radius to. I have had similar issues using "budget friendly" tools. However, when that is the issue it tends to be error in form and typically is less than .001" deviation.