pause and go in every nodes

[eondodge]

Good day guys,

Anyone experiencing a pause and go in every nodes in their machinning like mine? this results to chatter in cuts specially in arcs.

my gcode was generated from vectric vcarve 7.5 using masso postprocessor. As i've checked, there's nothing wrong with the gcodes as it uses G1 for straight segment and G3 for arcs (climb).

 

[breezy]

@eondodge,

What model MASSO do you have? And what version software are you running on it?

The Bicton Men's Shed 3DTEK Heavy Mill which has a MASSO G2 running ver3.44 and it pauses between changes in direction on arcs/circles. I was informed that backlash compensation was causing that. This pause results in small burn marks on the work piece, fortunately they can be sanded out.

I think there may be a test/beta version out for G3s that reduces the pause. Could be for plasma machines?????

Regards,

Arie.

 

[stevefrisby]

I have a feeling that I am experiencing the same issue, Never had an issue with my old controller. I am using v carve pro 10.

And if you have a machine designed to cut with accuracy sanding out what I would call a substantial marks is not an answer it is a work around

I will post photos eondodge can you let me know if this is what your talking about.

Btw I have sanded these with 80 grit, they are covered in this project but if i was cutting doors sanding them out would cause issues

Cheers

Steve

 

[cncnutz]

There could be up to 3 things at play that affect smoothness of motion.

1. Something to be aware of is that Masso uses Exact Stop machining not constant velocity. Constant velocity gives smoother motion by taking short cuts and making up the tool path on the fly. Exact Stop cuts exactly what is asked. Using constant velocity is the same as saying, cut me something that looks a little like this. The result is pieces that should fit together like a jigsaw puzzle piece won't.
   
2. The trap with Vcarce pro and Aspire is what looks like a curve to you of the Screen of Vectric software quite often isn't. There are 2 types of curves. Circular arcs and Bezier curves. The only curves that can be represented in Gcode is circular arcs. Bezier curves look like nice curves in Vectric software but are output as a series of straight lines. Before creating the final Gcode I do a conversion of all curves to Circular arcs. That way I get smooth motion similar to constant velocity. The advantage is that instead my cam software now makes the decision on the actual toolpath and I have total control over it, not the controller and if I need to make mating pieces they will fit together properly.
   
3. Backlash setting will cause hesitations when an axis changes direction since the motor has to stop and reverse direction. This is seen on curves and is unavoidable as the axis has to take up the slack in the drive train before it can start moving in the opposite direction.
   

The hesitation that Arie mentioned is related to turning on and off outputs in the middle of machining and turning on and off the THC in Plasma so won't be an issue here.

If you want to upload the Gcode file i can take a look and if EONDODGE uploaded his Vcarve Pro file I can have a closer look at it.

I only have aspire 9.5 so cannot open a version 10 file unfortunately but if my suggestion doesn't fix the issue Steve let me know and we can work something out. I can see the machine marks but can't tell if the surface is curved. I can look at the Gcode though.

Cheers Peter

 

[breezy]

Steve,

This is the project that paused on the arcs. The locations the pause occur is at the 90 deg points on the large circle. As these are picnic wine table tops, placing them in a jig on the lathe the edges can sanded and rounded over, which removes the marks. The marks are not so noticable on the smaller circles.

Regards,

Arie.

 

[stevefrisby]

Hi Peter I am pretty sure I understand, this is a big project and for some reason vectric did change the simple circles into parts, so what you are saying is that vectric has rather than cut one nice curve broken it into many and they don't line up. due to the size of the project it is a 4.8m wide addition to a stage going into mm to review the actual detail is challenging, i am basically using art based or small project based software to cut shop fitting parts. I will post a photo of size of the parts.

Hey did you have ant luck getting extra inputs added to the Masso input list? I am pretty bust atm but will be posting a mpg app soon with the relevant software and hardware diy solution I am hoping that by actually having a running add on Masso might give me the extra input assignments to make it a valuable toll and asset to the Masso community

Also I have a friend wanting to build a CNC I have convinced him to use a Masso controller, as I will probably end up being they guy building it and haven't got the time or energy to get mach3 and mach4 controllers running for him. He just wants something that works my issue is the cost of v carve I was wondering if you could suggest a cheaper alternative that is easy and has Masso post processor support.

 

[eondodge]

Quote from SteveFrisby on May 8, 2020, 8:42 pm

I have a feeling that I am experiencing the same issue, Never had an issue with my old controller. I am using v carve pro 10.

And if you have a machine designed to cut with accuracy sanding out what I would call a substantial marks is not an answer it is a work around

I will post photos eondodge can you let me know if this is what your talking about.

Btw I have sanded these with 80 grit, they are covered in this project but if i was cutting doors sanding them out would cause issues

Cheers

Steve

Hi Steve,

Your right, maybe we have same problem. Tried it also in our Chinese cnc with richauto controller and it cut smoothly.

Hi Peter @cncnutz,

Please see attached photo for the output, the pocket is cut roughly due to the stop and go motion in every nodes. Also attached the vcarve autogenerated toolpath with masso postprocessor. We are using node edits on designing mostly that results to bezier curves. Just don't know why the richauto can run this smoothly, maybe there's something in there that we can replicate. It shouldn't pause and go on the nodes.

Hoping to find some answers on how to resolve this issue.

 

[cncnutz]

Hi EONDODGE

Just looked at your Gcode and it is made up of a whole lot of G1 moves so that is your problem. Your curves are not circular arcs.

There are arcs in the Gcode but far too many G1's for something that is round.

Just spotted you are using bezier curves which are not true arc and will be output as lines. When you finish drawing convert the drawing to circular arc and output the Gcode. You will find the file much smaller and it will run smoothly.

Send me the Vcarve file if you like and I will have a look.

cheers Peter

 

[cncnutz]

Hi Steve,

I wrote an answer earlier today but it looks like it didn't post.

Vectric breaks circles up into 4 parts normally which you see when you go into node editing mode. When you look at Bezier curves and ovals they also look to be made up of arcs but they are not circular arcs so the Gcode is output as tiny straight lines as only circular arcs can be defined in Gcode. EONDODGE's Gcode file in the post above is a good example of arcs being output a lines. The result is a huge Gcode file, poor motion and tool marks.

For your friend

Vectric Cut2d You can use the existing V10 Aspire post processor on it and if not I can write one for it but I'm 99.99% sure it uses the same one.

Fusion 360 (free but has large learning curve)

Regards the input request there is no change to the previous reply from a couple of weeks ago. https://www.masso.com.au/forums/topic/a-home-switch-triggering-door-sensor/?part=2#postid-12293

I am keen to see the version 1 of your pendant.

Cheers Peter

 

[breezy]

Steve,

Put out a call out to TayloredTech about a low cost copy of Aspire.

Regards,

Arie.

 

[stevefrisby]

OK will do Thank you for your continued support Arie

 

[stevefrisby]

Dumb Question Arie but how do I reach out to anyone on the forum, is there a way to PM anyone? Honestly this it the first forum I have really engaged in (I like the respectful manner of the users of this forum)

Also have just realized that Vectric will chop up a nice circle when you use the offset function i have a screen shot of what it looks like I have a feeling this is why my CNC cuts looked as bad as they were

The lines with all the nodes were created as offsets from the nice circles

Cheers Steve

 

[Ross]

This might be not what you are asking help for. Not sure.

You can try this.

you have to join nods and reduce the number of nods.

I only have CorelDraw.

Ross

 

[cncnutz]

Hi Steve,

That is a great illustration of the problem. Your curve is made up of hundreds of straight lines instead of a handful of arcs.

Select the curve and use the Fit Curve Tool. Select Circular arcs and add a tolerance. Try 0.1mm to start with.

Have a look at the curve again and you will see that is is now a much nicer looking curve in node view and when you output the Gcode it will be a lot smaller and the machine will move smoothly because it is cutting arcs and not straight lines. Do not select Bezier curves which will give a similar looking curve to circular arcs in node view but the final Gcode output will be straight lines again as only circular arcs can be described in Gcode.

If you want feel free to post a DXF of the file here and I can show you what I mean. I have V9.5 so can't open a V10 Vcarve file.

Cheers Peter

 

[stevefrisby]

That's why I thought I would share this photo. Here is the new photo all i did was draw arcs with start and end point the same and center following the original arc and then deleted the original.

I didn't realize the use of the offset feature in Vectric did this so know in future to redraw any curves that it creates or just keep drawing circles and cut them as i did for this project

BTW this is a huge project.

I think this forum is a valuable resource to the Masso community so will continue to report success and problems

Btw Peter why did you not get the option to upgrade to 10, I am pretty sure I started with 9.5

Cheers Steve

 

[cncnutz]

Definitely looks like a big job Steve. Coming along nicely.

I usually skip a version unless there is some new feature that I really need. There are some nice improvements but nothing I need at present and at about $650 to upgrade, I think I can wait a bit longer.

Cheers Peter

 

[breezy]

@stevefrisby

Steve,

Dumb Question Arie but how do I reach out to anyone on the forum, is there a way to PM anyone?

It isn't possible to PM (private message) on this forum, but if you wish to contact someone use their @name as I have done at the beginning of this message and a You have been mentioned in a forum-post. email is sent to the registered email address of that person. If the discussion you wish with that person is to be private provide a spaced out email address for them to contact you on, don't provide a correctly formatted email address as phishing bots can extract them from the forum.

Regards,

Arie.

 

[eondodge]

Good day everyone,

I found a solution for this one already. stutter was eliminated and cutting has gone smoothly.

Using vcarve, go to edit and select "curve fit vectors."

select "circular arcs" to convert all your curves. it will also solve the very long G1 lines generated in output gcodes coz it will use the Arcs already (G3, I, J)