Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Forcing arcs into line segments for better accuracy?


Recommended Posts

22 minutes ago, Brad St. said:

interesting and all great feedback my quick question would be "how are they measuring the profile?"

it's easy to say a CMM but what if the probe is too large for the corner rad.....?

just asking 😃

We got one part that has gone back and forth for 5 months now. Programmed 4 parts all identically and 3 of the parts are coming out with .0002" true Position day and day out for the last 5 months. Part #4 is not and we have tried explaining it 10 different ways it is not being checked correctly. We even put the part on a surface plate and showed them that the holes are in line with .0002" they will not listen. The CMM keeps saying they are out .01" so fix the program. Program has been changed 10 times and the CMM results all repeat with .001 of each other off, but they still will not listen. 

Link to comment
Share on other sites

Yep, never argue with an inspector. if their numbers are not right they will be the next time you ask.

Alignments, alignments and alignments make a world of difference. Seen too many things to argue with em (even when I was one of them 😉

I was my own worst critic.

The item that is standing out to me is you've tried it many different ways and they are getting the same results in their inspection. that alone is making a statement to me that they are measuring it the same way as before. may not be correct but it's repetitive thus the measurement is looking for the same thing (right or wrong)

worst thing is measuring good parts bad and you go through what you are. of course if you measure bad parts good that's not going to help your reputation.

  • Like 2
Link to comment
Share on other sites
1 hour ago, Brad St. said:

Yep, never argue with an inspector. if their numbers are not right they will be the next time you ask.

Alignments, alignments and alignments make a world of difference. Seen too many things to argue with em (even when I was one of them 😉

I was my own worst critic.

The item that is standing out to me is you've tried it many different ways and they are getting the same results in their inspection. that alone is making a statement to me that they are measuring it the same way as before. may not be correct but it's repetitive thus the measurement is looking for the same thing (right or wrong)

worst thing is measuring good parts bad and you go through what you are. of course if you measure bad parts good that's not going to help your reputation.

I was in Malaysia years ago and good parts were being called bad. I took 3 different measuring tools and measured the features they were calling bad and went to inspection and they started trying to explain the problems to me. I said let me see your Nominals in which your doing your inspections to. They said that is not allowed and I went and got the main plant foreman and told him the whole project was on hold until they got me the nominal CMM reports. They gave them to me and 6 months of parts had been rejected because someone had gone in and changed the nominal values of the CMM program. We got them corrected and every single feature on the parts were good. They went back and pulled the 6 months of scrap parts and they were also good.

  • Like 2
  • Huh? 1
Link to comment
Share on other sites
3 hours ago, pro grammer said:

Force your arcs into quadrants and use G60.

I've only ever used G60 when drilling. I'm curious as to how would that function would help in circle interpolation? I ask because the function needs an overrun distance and if you overrun an arc, now you're running into arc centerpoint tolerance problems.

2 hours ago, Leon82 said:

It's an option I believe as ours say invalid gcode when we try it

Try it in MDI by itself. I haven't used it in years.

Link to comment
Share on other sites

So just an update on this project,

I applied G131 P3 (on my machine I have P3 slider all the way to accuracy) onto all my finishing toolpaths, and also broke all arcs into line segments of about .0008 with smoothing controls, .0002 overall tolerance. I set all the opti-rough toolpaths to G131 M3, as well as any of the other toolpaths that had helical moves. 

The next part ran with these settings, only 5 arcs failed on the profile tolerance, out of about 30-40 such internal corners. This was without slowing down feed, or adding spring cuts, or rest machining. I noticed too that many of the endmills that I had wear comps on to bring features on size, I had to take the wear comp out because they were now cutting much more closely to how they were programmed. by comparison, my original toolpaths, before any of these settings, G131 P/M or R, pretty much every arc on this part was failing on the profile, So I would say these settings made a huge difference, and will definitely be setup on all toolpaths moving forward. 

For those asking about the inspection, this is being done with a brand new Zeiss Accura CMM with scanning head and 1mm tip. 

 

  • Like 1
Link to comment
Share on other sites

Is the viewing department (Inspection/QA) checking by profile tolerance direct to the CAD model, or are they actually calculating rad centre points?

Checking direct to the model is the most accurate way for partial rads - but if you have a print where the jockey has dimensioned rad centre points, and then tied this right down, you could be in trouble.

Here's a quick explanation of how a eenyweeny bit of error means BIG deviation:-

Capture.JPG

  • Like 1
Link to comment
Share on other sites
On 6/12/2020 at 8:38 AM, crazy^millman said:

Try getting a 7 flute endmill and take the same cut the difference will be night and day.

Just to add to Ron's physics lesson, the other thing additional flutes give you is more continuous engagement of the flutes.

This results in a more stable cut as there is always at least a couple of flutes engaged even on a light radial cut. 

A three flute endmill might only have a single flute engaged and the cutter can start to bounce. In the corners with extra material the 3 flutes are just overwhelmed and deflect. More engagement can prevent both of these conditions.

As with everything machining it is a matter of balance. We do a lot of unsupported 4 axis work and we often "tune" cutter paths by changing the number of flutes on the cutter. Balancing the tool pressure with the chip formation through the whole cut is the goal.

  • Like 2
Link to comment
Share on other sites
12 hours ago, machineimpossible said:

For those asking about the inspection, this is being done with a brand new Zeiss Accura CMM with scanning head and 1mm tip.

If not being measure correctly that means nothing. What are the points collected being measure back to? What does the Nominal model information have and how was it modeled? Was the model made to the nominal mean or the low or high mean? Is it a DPD/MBD process where model verification was down with an external program for integrity checks when the model was imported into the CMM Software?

I was in one place complaining about True Position being wrong on a part. I measured them with PCMM and found most of the holes were .005 to .007 out of round. The inspector argued with me that made no difference that the true position was the true position the way he was measuring it. They were not checking roundness just 4 points at each side of the hole and that is how they were checking true position of the features. I then tried to explain that True Position of a hole is a cylindrical feature where the axis of the feature is compared back to the axis of the nominal feature to make sure the cylindrical zone is within the true position tolerance. He then came back with the surfaces around it have .02 profile so that changes. He was the first inspector to ever argue for a floating Datum structure. I went back and proved my case 5 different ways the part was programmed correctly and they were inspecting it wrong. They didn't want to hear it make it pass inspection and I walked away and told them no I cannot and will not be a part of it. I lost the customer and not sure what came of the whole situation. Point is as much as many people think they understand inspection and the correct way to check parts they don't. A lot of time they are just button jockeys not sure of the correct way to measure something. Holes were out of round because they were putting the same part back in the machine and not indicating the 2 datum holes in to keep re cutting the part to take back to inspection.

1 hour ago, nickbe10 said:

Just to add to Ron's physics lesson, the other thing additional flutes give you is more continuous engagement of the flutes.

This results in a more stable cut as there is always at least a couple of flutes engaged even on a light radial cut. 

A three flute endmill might only have a single flute engaged and the cutter can start to bounce. In the corners with extra material the 3 flutes are just overwhelmed and deflect. More engagement can prevent both of these conditions.

As with everything machining it is a matter of balance. We do a lot of unsupported 4 axis work and we often "tune" cutter paths by changing the number of flutes on the cutter. Balancing the tool pressure with the chip formation through the whole cut is the goal.

Yes that is the other part of more flutes I didn't mention. Thank you for helping to point that out.

  • Like 1
Link to comment
Share on other sites
22 hours ago, machineimpossible said:

So just an update on this project,

I applied G131 P3 (on my machine I have P3 slider all the way to accuracy) onto all my finishing toolpaths, and also broke all arcs into line segments of about .0008 with smoothing controls, .0002 overall tolerance. I set all the opti-rough toolpaths to G131 M3, as well as any of the other toolpaths that had helical moves.

Typically I'll only use M1 with Opti-Rough because as the toolpath name implies "...Rough". I'll run 1's on my modes if I only need to hold around 25µm or so. I'll use 2's if I need to hold 10µm or so and 3 ONLY on finishing passes if I need to hold single digit µm.

You finish the paths, I'm certain they'll ALL pass... as long as inspection does their job. :rofl:

:coffee:

See the attached document.

Matsuura High Speed Look-Ahead Functions Procedure.pdf

13 hours ago, Newbeeee™ said:

Is the viewing department (Inspection/QA) checking by profile tolerance direct to the CAD model, or are they actually calculating rad centre points?

Dollars to donuts they are checking by calculating radius centER. :P

:thumbup:

:coffee:

Link to comment
Share on other sites

So the inspection is being done right from the solid model as nominal. I cannot speak to any import/conversion issues with the CMM software bringing the model in. The format we were supplied from the customer was .STP but I don't know if that went right into the CMM software with no issue, or if it needed to be converted to something else.

As to the method, they are using full scanning for everything, not just minimal points. so each of these internal arc features are scanned with dozens of points all along and across the feature. So I would say they are being checked as true partial cylinders, and the CMM is report deviations of Form, Position and Size to the solid model as nominal.  Which of course is required to truly evaluate a profile of surface tolerance.

  • Like 1
Link to comment
Share on other sites
2 hours ago, machineimpossible said:

So the inspection is being done right from the solid model as nominal. I cannot speak to any import/conversion issues with the CMM software bringing the model in. The format we were supplied from the customer was .STP but I don't know if that went right into the CMM software with no issue, or if it needed to be converted to something else.

As to the method, they are using full scanning for everything, not just minimal points. so each of these internal arc features are scanned with dozens of points all along and across the feature. So I would say they are being checked as true partial cylinders, and the CMM is report deviations of Form, Position and Size to the solid model as nominal.  Which of course is required to truly evaluate a profile of surface tolerance.

Good enough for me. Press on and good luck getting your process dialed it to make the best parts possible.

  • Like 1
Link to comment
Share on other sites
On 6/12/2020 at 8:16 AM, machineimpossible said:

The component I am working on has an overall profile tolerance of .005 to the entire model. There are dozens of small internal corners, all normal 90 deg arcs. Most of these arcs are falling out of tolerance on the .005 profile.

You should be able to hold .005 profile easily.  The little tricks mentioned are for when your splitting tenths.  Looks to me like the machine needs looked at. 

When was the last time it was checked (ballbar, laser,etc.)?  What were the specs?

Link to comment
Share on other sites
3 hours ago, machineimpossible said:

So the inspection is being done right from the solid model as nominal. I cannot speak to any import/conversion issues with the CMM software bringing the model in. The format we were supplied from the customer was .STP but I don't know if that went right into the CMM software with no issue, or if it needed to be converted to something else.

As to the method, they are using full scanning for everything, not just minimal points. so each of these internal arc features are scanned with dozens of points all along and across the feature. So I would say they are being checked as true partial cylinders, and the CMM is report deviations of Form, Position and Size to the solid model as nominal.  Which of course is required to truly evaluate a profile of surface tolerance.

I have had issues with inspection scanning profiles and giving bad data on small arcs. 

On one part they used a 1/2mm ruby to scan a profile with an .011 inch radius and a .0003 inch all around profile tol and said I was out at in two spots.  Well, the center of the probe tip was whipping a .001 inch arc and which has the same effect as with an endmill.  After chasing my tail for four weeks, they finally switch to a smaller (.2mm) tip, took measured points and voila, wouldn't you know the parts were good all along.

Link to comment
Share on other sites

See if you can get a graphical output of the scan with images of the outlier points or areas that are out of spec. That will help you dial in on if it's the machine or the inspection. What Matt stated above is what's been on my mind all along. They sound like their doing the right process but just like cnc programming tool selection is crucial for the right results.

  • Like 3
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...