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:

Surface Quality


LucasGC
 Share

Recommended Posts

12 minutes ago, LucasGC said:

oh shoot, was looking in mcam config - now i see you're in control def. Thanks, will try this now. 

Yeah control def.  You don't need cimco per say, but in this case you are able to use cimco to visualize the output code, which is helpful.

I personally hate the canned responses from MTB's on customers having to learn thing for themselves....  If they just understood that if they were to put a little effort into support in these cases, say having someone on staff that is a subject matter expert, than they would sell more machines through raving reviews, not to mention they would prop up the industry through education on faster and better practices for programming.

Link to comment
Share on other sites
13 minutes ago, huskermcdoogle said:

Yeah control def.  You don't need cimco per say, but in this case you are able to use cimco to visualize the output code, which is helpful.

I personally hate the canned responses from MTB's on customers having to learn thing for themselves....  If they just understood that if they were to put a little effort into support in these cases, say having someone on staff that is a subject matter expert, than they would sell more machines through raving reviews, not to mention they would prop up the industry through education on faster and better practices for programming.

I agree, i was very disappointed with this response. And they sure never said anything about changing this tolerance value. I emailed them saying I was going to change it hoping for a 'oh yes it should have been that way to begin with' or 'well that might cause problems with something else' - but more or less just got an 'okay'.

This changed helped a lot, thank you. it does still studder step a little bit, which is strange to me since it's just a roughing toolpath.

I'm thinking I still want the cimco for the convenience, and it still seems to me the post is breaking down the toolpath smaller than what i'm seeing on mcam - why else would there be studder steps where I'm seeing smooth curves? when i backplot i see the curve only having two points, which makes me think it's an arc, but i guess it could be a spline.

 

Anyway, much better, could be a little better

thanks a ton

Link to comment
Share on other sites
23 minutes ago, LucasGC said:

So it's jittery because the post only creates arcs in the major planes. are all 5-ax machines like this?

No and like I have said many times before I have done good work on the Thermwoods 5 Axis machines so there is something going on that I am sorry to say you are going ot have to figured out for everyone else. Been pretty much my career figuring out and doing what others didn't want to our couldn't. Not meant in an arrogant way more of the I am determined enough to figure out a way and get it done. If it can be done then you will get it figured out and you have already done a lot of leg work and think once you get the right combination down you will be very happy with your results.

Link to comment
Share on other sites
15 hours ago, C^Millman said:

No and like I have said many times before I have done good work on the Thermwoods 5 Axis machines so there is something going on that I am sorry to say you are going ot have to figured out for everyone else. Been pretty much my career figuring out and doing what others didn't want to our couldn't. Not meant in an arrogant way more of the I am determined enough to figure out a way and get it done. If it can be done then you will get it figured out and you have already done a lot of leg work and think once you get the right combination down you will be very happy with your results.

Hey, thanks. No worries, i think the most of the problem was that the tolerances weren't the same between mcam and post.

I didn't know if i should be able to make arcs in other planes, so it's good to know i can't and that they will definitely be split into lines. this explains the jagged steps, it was just not what i was seeing in mcam. 

I am a bit confused about what i'm seeing in mcam vs what i post out and what i would see in cimco edit. If i have my tolerances the same as in the post, then other than my arcs in non-major planes and c unwinds shouldn't i be seeing the same thing? 

I'd also like to know some things about the geometry the machine can handle, this will be my next email. such as, what's the minimum size radius the machine can run through before slowing down, and if i have my tangency factor set to 10, what should i set my break angle to to avoid sharp corners

Link to comment
Share on other sites
18 hours ago, C^Millman said:

No and like I have said many times before I have done good work on the Thermwoods 5 Axis machines so there is something going on that I am sorry to say you are going ot have to figured out for everyone else. Been pretty much my career figuring out and doing what others didn't want to our couldn't. Not meant in an arrogant way more of the I am determined enough to figure out a way and get it done. If it can be done then you will get it figured out and you have already done a lot of leg work and think once you get the right combination down you will be very happy with your results.

Did you ever have to change your mcam tolerance to match your post tolerance? the standard units match, but metric has different values. I asked them about this and why this was and just got the reply that different machines work differently and this is a common 5 ax post for all, i just don't know what the advantage of having different tolerance values would be between post and mcam.

Was also told the tangency equation is proprietary, and i'm guessing so is minimum arc radius - bummer...

Does anyone know if there is a way to tell mcam to break arcs into lines during toolpath creation in non-major planes? I would like to do this because i think it will give me a closer representation of what the post will look like

Link to comment
Share on other sites
9 minutes ago, LucasGC said:

Did you ever have to change your mcam tolerance to match your post tolerance? the standard units match, but metric has different values. I asked them about this and why this was and just got the reply that different machines work differently and this is a common 5 ax post for all, i just don't know what the advantage of having different tolerance values would be between post and mcam.

Was also told the tangency equation is proprietary, and i'm guessing so is minimum arc radius - bummer...

Does anyone know if there is a way to tell mcam to break arcs into lines during toolpath creation in non-major planes? I would like to do this because i think it will give me a closer representation of what the post will look like

Control Definition should do this you can change this to never output arc and what that should do it send the information to Post to linearize everything if the post is tied to the MMD and CMD. If not then you will have to look in the post and see if there are setting in that post to make the changes.

I have seen their Logic for the Tangency Factors and funny how some think a basic accel/decel calculation is rocket science.

Link to comment
Share on other sites
29 minutes ago, C^Millman said:

Control Definition should do this you can change this to never output arc and what that should do it send the information to Post to linearize everything if the post is tied to the MMD and CMD. If not then you will have to look in the post and see if there are setting in that post to make the changes.

I have seen their Logic for the Tangency Factors and funny how some think a basic accel/decel calculation is rocket science.

It would be so nice to have... 

I think you might be thinking about breaking down arcs differently than how i mean it - my post already breaks down all my arcs in non major planes - mcam toolpath creation does not. If i backplot my toolpath and save it as geometry, there are still arcs. what i want is for that arc geometry in mcam to be broken into lines

Link to comment
Share on other sites
41 minutes ago, LucasGC said:

It would be so nice to have... 

I think you might be thinking about breaking down arcs differently than how i mean it - my post already breaks down all my arcs in non major planes - mcam toolpath creation does not. If i backplot my toolpath and save it as geometry, there are still arcs. what i want is for that arc geometry in mcam to be broken into lines

That is a different and has no bearing on what the post will output. You are over thinking it and there is no real need to have backplotted geometry in Mastercam match what the NC code is. They can be two different things, but still be what you need at the machine. The post is your translator so to speak to take English, French, Greek, Spanish, Russian and covert it to a usable format for the machine. The CAM is not the same as the NC. The NC can be backplotted like you have seen with CIMCO, but I only trust the CIMCO so far as it cannot match 100% what you get on a 5 Axis machine. 3 and 4 Axis to a point, but for 5 Axis you need to use a true 100% CAV to get the best idea what you post is giving you for output.

Link to comment
Share on other sites
23 minutes ago, C^Millman said:

That is a different and has no bearing on what the post will output. You are over thinking it and there is no real need to have backplotted geometry in Mastercam match what the NC code is. They can be two different things, but still be what you need at the machine. The post is your translator so to speak to take English, French, Greek, Spanish, Russian and covert it to a usable format for the machine. The CAM is not the same as the NC. The NC can be backplotted like you have seen with CIMCO, but I only trust the CIMCO so far as it cannot match 100% what you get on a 5 Axis machine. 3 and 4 Axis to a point, but for 5 Axis you need to use a true 100% CAV to get the best idea what you post is giving you for output.

I understand it won't affect the post, I'm just trying to get my mcam as close to what i would see in cimco edit as i can, even if it's not perfect

Link to comment
Share on other sites

I've been experimenting with making toolpaths on the same part in both metric and standard, i started using the same values - .01mm tolerance / .0004" tol.

I noticed right away there was at least a difference, i've been working on smoothing out the standard since. If I can get it to where I want it then at least i know it will be problem with my metric values in the post (right?)

The standard will move through the points much faster, to the point where it does make some jerky moves, but at least it's fast. Lowering the tolerance to .0001 has helped, plan to go even smaller, and adjusting the tan factor i think will dial it in.

  • Like 1
Link to comment
Share on other sites

Alright, this is it. Did a test, confirmed it was being in metric rather than standard that was causing problems, hopefully this means it is in the post and will be fixed soon.

This is the email I sent, i hope it is in depth enough:

Okay so i did some more testing, I was curious if the metric vs. standard defaults were the same, so I made a part in mcam in both standard and metric, same part, and used the same toolpath with equal value settings. (.01mm = .0004in)
When I ran this on the machine i did see a drastic difference - the standard was much faster.
I decided to try to dial in the standard toolpath since i haven't been able to dial in the metric - and I was able to.

I made the same changes to the metric file for every test so i have a comparison, i even compare the metric with chordal dev. in control definition between .00127 (default in post) and .00001 (default in control definition). {It seems the post value does not overwrite the mcam value}.
The standard outperforms the metric in every test - at least twice as fast.
The best settings I got with the standard were at .00004 total tol, and 40 tang - though it worked fine at 30 and 20, was a little jittery at 10 - made it furthest at 40- is there a drawback to using max tangency other than tolerance deviation?
I made 9 videos, each 30 seconds so you can tell how far it got at each setting, the only setting changed between videos is tan. factor. The two important ones are video 3 and video 6
 
This is a very big difference and i do not know where it's coming from.
Please, can you help me resolve this?
I am attaching 14 files, let me know if you do not get them all.

I added the "{It seems the post value does not overwrite the mcam value}."

Because I had been asking them about it and was not getting an answer, until I got an answer that did not match my result:

I still think changing the tolerance in the control to match the value in the post is helping a lot. Is this the way it should have been from the start or was there a reason to have different values?
Different customers need different settings for different materials on different machines. The post is a general post designed for all our 5 axis machines.  Model 90's will run differently that model 70's.  

I was really hoping for the reason so i can know what affect it will have. It really seems like these values should have been equal, just because the standard units are equal, and I don't understand why changing to metric would require these to be different. If there is an advantage to having different values, I'd like to know what that is.

Customers use the post one to overwrite the mastercam one.

Only going to attach vids 3 and 6

3.3gp

6.3gp

Link to comment
Share on other sites
1 hour ago, C^Millman said:

That is why I never had the problems you are having as I always ran them in inch. Excellent work sir.

That honestly means a lot, haha. No one at my work really understands my problem because I am the only one running the CNC. 

 

This is the response I got, I don't think it's related.

there is no other drawback to having a high tangency besides the deviation.  What you are seeing in your videos most likely is the control Starving for motion because your segments are too small.  If you can only process 30,000 commands a second and your average line segment length is .002 (.06mm), you will only be able to run an average of 60 inches per minute, or 1,524mm per minute. 

I tried these toolpaths with bigger tolerances to start, and tightened them from there, so I really don't think it has to do with segment length. Especially because my tolerance is set to equal values for both (.001mm = .0004in) so I'd think they would have equal segment lengths.

Link to comment
Share on other sites

Just a thought...

go back to your pocket program.

 

I would not use high speed on that router.....a mill...ok...but a router....no.

just for fun make a pocket toolpath with a constant spiral,   turn on finish pass....

SET G09F1

SET G08F1

Set the tool off to the side and cut air and see if the machine speeds up.

 

I have not found anywhere on the internet where FORMAT for arc acel/decel default is G08XX.

Everything for Thermwood 70 says format has an "F" just like tangency factor format.

Your post sets default arc acel/decel to : G0800...If this is actually correct for your

particular control, have you tried G0801?

 

I also read in another post from Practical Machinist if the tangency factor was set beyond 8 you could experience unpredictable results.

But the Gcode list says 1-40...one list says 1-20....

 

 

 

G Codes Supported

G00               Rapid traverse. Rapid traverse uses linear interpolation at rapid transverse speeds on the SuperControl. Will produce a straight line.

G01               Linear Interpolation. The information contained in the block is used to produce a straight line at a specified rate.

G02               Circular Interpolation Clockwise. All four values must be listed. The I, J, and K values should be incremental.

G03               Circular Interpolation Counterclockwise. All four values must be listed. The I, J, and K values should be incremental.

G04F             Dwell time in seconds (3.1 format).

G05               Spline Marker - Begin Spline.

G06               Spline Marker - End Spline.

G07               Undefined.

G08F#        Arc Factor. Sets maximum circular speed.  F values are integers valid from 0.1 up to 5.  The machine defaults to G08F1 upon power-up. Ensure that if the maximum circular speed-factor is changed in the program that the factor is returned to F1 at the end of the program. The systems current setting for Arc Factor can be viewed by pressing ctrl + t (the dialog will appear for 10 seconds).

G09F#          Tangency Factor. F values are integers valid up to 40. Machine defaults to G09F1 upon power up. Ensure that if the tangency factor is changed in the program that the factor is returned to F1 at the end of the program. The systems current setting for Tangency Factor can be viewed by pressing ctrl + t (the dialog will appear for 10 seconds).

G10               Cancels Mirror Function for incremental style programs. Be sure to return the mirrored axes to the position it was at when the mirror command was first issued before disabling with a G11.

G11               Mirror Function. Reverses the direction of motion of the listed axes. This works best with incremental programs. If cutter compensation is being used within the mirrored commands the tool path will be on the opposite side of the tool path. Sample; G11X or G11XY

G12               90° Clockwise Ellipse.

G13               90° Counter-Clockwise Ellipse.

G14-G16     Undefined.

G17               XY Plane selection for Cutter Compensation.

 

Hard to tell without seeing the code but, if it is a software/nc code issue than there are two things that I would check - Forrest's G09 is one...

===
Forrest is referring to the "TANGENCY FACTOR" and the format is G09F##, where ## represents 1 through 20. The default on the machines is usually 1.

The Tangency Factor on the older machines (Pre-Smoothing G07F##) set the threshold at which the machine would consider two entities tangential and thereby not coming to a stop, but instead combining the entities into the same motion/velocity curve.

Normally you do not need to increase the default as most software will create tangential line and arc segments when possible. You will see a Tangency Factor of 3-5 when you have 3d surface modeling where the toolpath is made up of small line segments with very small angle changes that are not tangent but that you would like the machine to "flow" through as it they were. Any angel change larger than the threshold set by the Tangency Factor will still cause the machine to come to a decelerated stop and then an accelerated start in the new direction.

You may want to check to see if someone has added a G09F## with some "stupidly large" value that would have increased the tangency threshold to the point that the 90 direction changes would be attempted without stop and start at the corner.

====
Another thing to check is: IF the program generating the code has placed arc moves in the corners in order to "roll" the tool around each while still producing a square corner - then you should check for the presence of the ARC SPEED FACTOR parameter - G08F##. This commands numeric parameter increases or decreases the default "speed control" that is applied to tangential arcs. The control by default has a calculation built in the will automatically adjust the velocity of the machine as it goes through arcs. This adjustment is based on the size of the arc radius. IF the radius is large, then there may not be any decrease in speed. But as the arc gets smaller and smaller (the smaller the arc the more "instantaneous" the direction chance gets), the controller will automatically decrease the speed in the arc - decelerating as it approaches it and then accelerating back up to speed as it leaves it.

A numeric parameter is like a multiplier for the built in calculations. 1 is the default (calculate as usual) and should normally be fine and you do not have to explicitly define the G08F1. If you want to reduce the arc velocity you would use a multiplier less than one (<1). G08F0.5 will halve the natural velocity adjustment calculations of ALL arcs that follow. If the parameter is larger than 1 (>1), then this means that the velocity calculations would result in increased values. G0F2 would double the default calculations.

You may want to check for a G08F## with a number/parameter greater that 1.

===

Both of the G09F## and G08F## parameters do not need to be explicitly defined in the NC code if the defaults are all that are required. (Which is in most applications is all that is required.)

  • Like 2
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...