Smoothing gone?

[kretallick144]

I have the latest update,  But now trying to get a Lathe program going i cannot find a box for smoothing anywhere!

It is in my previous codes, but not the new one.  Using a Fanuc turning post processor.

I end up with a large code missing most of the G2/G3 radi.  Lots of short moves.  Im not even going to try and run it in the machine.

No checkbox in either the toolpath setup or the post processor....

Another Glitch?

[seth.madore]

I don't think Smoothing existed in the Turning toolpaths before this last update...

[akash.kamoolkar]

@kretallick144 the new turn profile roughing and finishing strategies never had a smoothing parameter. You can, however, enable smoothing in the spun profile in the setup dialog. If that does not work perhaps you could attach your file here and we could take a look. As a temporary workaround you could use the legacy turn profiling strategy since it has that parameter.

Regards,

Akash Kamoolkar

[kretallick144]

Maybe there never was smoothing, was sure i seen it previously.  There is in grooving.

Spun profile smoothing errors the profile paths with a No valid turing profile found.

[kretallick144]

I have checked radius arcs is ON.

I have no idea why it is not using G2/G3 as per all other codes i have done.

Anyone have any ideas?

[Anonymous]

I set origin at model face, changed from "tip" to "tip tangent", added finish profile operation and posted it with generic Fanuc turning post, I get arcs so problem is in your post.

[kretallick144]

VicKosta, Thankyou for taking a look.

Something strange going on.    I had a finishing profile in mine, was it visible when you open the file? 

I posted your toolpath but the finishing had the error No valid turning profile found.

Actual code was fine otherwise, Arcs were present.

I deleted and made a new setup and toolpaths but an still missing the Arcs.   Is it possible the post processor is corrupted somehow?

When you say problem is in my post do you mean the Post processor?   Im using the same Fanuc turning one i have used for nearly 2 years.

[kretallick144]

OK, i ran yours again an the problem is back.

I reinstalled the Fanuc turning post processor but still no luck.

[Anonymous]

I think I deleted your finish profile in course of trying to find out where the problem is and then forgot about it, my bad.

Now, I played with two files to compare results, if I post your original file using same Fanuc turning post, freshly downloaded from HSM library, I don't get a single arc move.

Next I moved origin in setup to model top and reposted, got all arc moves but there is another problem, choice of "tip" in tool definition.

Tip as defined by AD is intersection point of insert side angles, which changes with different geometry inserts, 35 degree diamond being the worst case scenario.

I tried to explain this to AD long time ago, nobody listened and nonsense is still there.

There is no such thing in any other software I used before, and there is no such thing in practise, look at the compared tool paths after I set tip to "tip tangent", ignore the dotted lines, feed rates exceeds those set in plotter as feed moves.

In simulation you don't see any errors but when you post, resulting coordinates are way off from part geometry, primarily in X axis but also in Z axis.

This means that when you touch off your tool, you would have to offset it back by value of discrepancy or crash your tool and scrap first piece.

@akash.kamoolkar , why is this still part of the package ?, it has no functional purpose that cannot be substituted by tip tangent or tip center point.

I plotted each file with graphic profile retained on screen for comparison.

Lower profile is result of "tip" and upper profile is result of "tip tangent"

Below is a result from your original finish profile with origin set at stock top, you should be able to set your origin in setup to model top and get arcs in posted file just as I did.

So the post is not a problem, it seems to be placement of origin in setup, I also practise making a sketch of sectional profile in file, if it's not there I add it to file because at times, tool paths fail if sketch of sectional profile is not there.

In this case not having sketch of profile doesn't seem to play a role but you cannot do any damage by including it,..... it should avoid that.... "no usable profile found" .... error.

I start all turning jobs with sketch revolved around Z axis to create model, origin is always model top and I don't recall having numerous issues other people have in a long, .... long time.

I add sketch of sectional profile to all customer supplied models before moving on to programming stage.

[akash.kamoolkar · Accepted solution]

@kretallick144 We are working on improving the spun profile algorithm but you can turn on the new version by checking the "spun profile" flag in preferences->preview features. When i turned it on, then turned on smoothing in the setup and regenerated the toolpath I got far fewer lines in the program. You can play around with the smoothing tolerance value in the setup if you want fewer lines of code.

Regards,

Akash Kamoolkar

[Anonymous]

Look at my previous post carefully because I am actually trying to help you and anybody who uses "tip" in turning tool definition without being aware of problem it creates.

Tip, as defined in Mastercam, is applicable in using round insert and it conforms to standard definition of tips orientation in CNC lathe programming manuals in existence for decades, Fusion "tip" would be valid option if used as number 5,6,7 and 8 in diagram below but only with round insert.

There is no such thing as tip defined by intersection of insert geometry angles, this is only present in Fusion, programmed point needs to be in sink with how tools are touched off at the machine, meaning contact points at surfaces parallel with X and Z axis.

So "tangent point" is defined as point of intersection between vertical and horizontal line when insert tip is touching both lines and is referred to as "imaginary programmed point" in many books and manuals.

In machine, horizontal and vertical lines are diameters parallel with Z axis and faces parallel with X axis.

This is valid for all types of inserts regardless of geometry when used in combination with "in computer" cutter compensation.

Using 80, 55 and 35 degree diamond inserts with "tip" in tool definition produces different margin of error because tip is intersection of insert side angles and has no useful purpose with these types of inserts.

As stated, "tip" has limited functionality that is easily substituted by "tip tangent" and therefore absolutely useless option.

I would hope that in face of obvious, "tip" would at least be restricted to use with round insert and nothing else but this has been ignored for a very long time and any attempt to deal with it is ignored by same people who put out surveys asking people to help them improve turning section of Fusion.

It took over a year that I am aware of to take constant surface speed out of threading in turning so no surprise but one thing stands out here.

If this is supposed to promote Fusion as being more versatile it's only showing immaturity and ignorance.  

People want stable, dependable, sophisticated product that they can rely on. Instability, crashes, monthly agitation with updates (and setbacks), lock of refinement and ignorance are not very appealing in comparison with established products that Fusion is aiming to compete with.

From images below, it seems Fusion has invented tip #10, which as shown further up in my previous post, is equivalent of leaving loaded gun on coffee table and telling kids not to touch it, what can possibly go wrong?

[akash.kamoolkar]

@Anonymous I understand the point you're making and trust me we haven't forgotten about this request. Unfortunately we just do not have the resources to prioritize this project right now.

Regards,

Akash Kamoolkar

[Anonymous]

I can help you with some technical issues but I can't be asked to fill the surveys and then come across this nonsense, you guys need to put your house in order, you are tinkering with a lot of businesses and professionals out here who demand better than that for daily operations, safety at work, preserving equipment and getting things done on time and in line with requirements.

If this is all about hobbies then carry on, it's almost fun at times. 

[kretallick144]

VicKosta,

I tried moving the origin but there was no difference.

akash, Thankyou!  that solved the problem!  But why did it appear suddenly?  ive been doing the same thing for many designs and only had is happen now,  Are the updates resetting things without us being notified? 

VicKosta,   Thankyou for all your time! appreciated greatly.

I think we have spoken before on the tool tip issue. it does make things harder for people with limited experience.

The tip issue could be why im having to change offsets or machining limits on the model to get the required dimensions.  A trap for us newbies.  It cant be that hard to remove all the setup choices and leave only  the required industry standard one can it?   Im tying to build a business and yes these hiccups that appear slow things down.

Ive said once before, Fusion is good but very glitchy! We pay real money for it, should get consistent real results.

[Anonymous]

Moving origin to model face was really in combination with other settings I made that are in line with how I work.

I always use model face as origin, that is Z0 when posted and all work is referenced from there, machine origin is set to same place on part, that point is finished face of part and center line, not stock face.

I also checked spun profile and smoothing in setup, after I made few adjustments, I got all arcs in code, I have routines that work, I avoid traps built into Fusion and try to make others aware of them. 

Lathe section of CAM lacks many features that you can find in established packages, it drifts between model and sketch when in reality all lathe work can be programmed on 2D sketch as has been done for decades.

Fusion has good features too, like ability to peck in turning, great for copper and plastics, grooving locks refinement, so does threading, ID threading is called face threading when selecting holder, confuses the hell out of people, face grooving tool holder have strait blade, it crashes into part as you attempt to make a groove, there are numerous things that never get fixed and to say that there are no resources to deal with operant need is ridiculous, get some help AD.

Frequent crashes get on my nerv, it's paid software, not beta, it needs to be stable, proficient, productive, intuitive, 

progressively better in everything it does, but it seems that we are the beta testers and as soon as something goes stable it becomes manufacturing extension that adds cost on top of subscription, not funny at all.

If I was building business I'd have something on side to use when SHTF with updates or when internet is down.

Last time my home internet was down, Fusion took over 5 minutes to load, not very practical.

And, finally, yes I think we deserve better then can of worms without lid, professional or beginner, same good money

[Anonymous]

I just downloaded file that I first posted in response to your post, I also uploaded NC file showing all arc moves in finish profile at that time and I pointed out which post I used.

Now I posted entire file and there is no sign of anything being out of place except that my finish profile did not extend past groove shoulder, I set tool to tip tangent and all other settings that contributed to producing right result and yet, you did not find that wordy of solution, .... just curious as to why?

[Anonymous]

Never mind, I know why.