Square Profile - isn't !!

[JG]

I don't do a great deal of work in CamBam - but I'm grateful that I have the option !!

I can normally fathom out what I've done wrong when something happens that is not what I anticipate but today I've found an issue that doesn't make sense - to ME.

The job is a very simple 'Profile' 35.5mm wide, 20mm high, 3mm with two tabs cut with a 1.5mm end-mill in Ash. I'll attach a photo of the result along with a screen-shot of the CamBam Tool Path and the G-Code created (and used!)

The 'issue' is that only one of the corners is 'square' - bottom left in the photo - which is the starting point of the path. The other three corners are rounded and I'm sure you'll see from the screen shot that I have not specified this - more importantly I haven't specified anything in the CamBam profile that I can see would make the G-Code call for it.

Perhaps the greater wisdom that you all have can shed some light on the anomily?

[pixelmaker]

It could be that the controller uses a constant velocity setting for the three radii. If this setting causes this to happen, it never occurs at the start and end points of the milling process, which is why only three corners are rounded.           

https://youtu.be/XT2Jq76NChM?feature=shared

[lloydsp]

It also might be because the actual tool diameter is different than that specified in the MOp.

In order to cut a square corner, CB must plan a curved path with the tool's surface being the 'pivot point' of the curve.  If the tool diameter doesn't match the MOp, you'll get that.

Lloyd

[EddyCurrent]

I'm going with Polyline13 not forming a closed rectangle, i.e. it does not join at the 'square' corner.

[JG]

Bingo!  - though I haven't yet changed the setting -  I'm sure that will be the answer, I'm back in my office/design suite   and the copy of Mach3 is in the Workshop (of course)

At least I now have something to work on - thanks @pixelmaker.

I usually do have rounded corners (unless I'm cutting straight lines!) so hadn't noticed this effect previously. The issue about speed - ie. that Exact Stop will be the slowest option - is irrelevant as far as I'm concerned; I'm not working commercially.

[JG]

It also might be because the actual tool diameter is different than that specified in the MOp.

In order to cut a square corner, CB must plan a curved path with the tool's surface being the 'pivot point' of the curve.  If the tool diameter doesn't match the MOp, you'll get that.

Lloyd

Thanks for the input Lloyd, but as you'll now see (from my response) @Pixelmaker has the solution in one

I'm extremely pedantic in making sure that tool diameters specified do match those used and am well aware of the consequenses of any mis-match - but it's a valid point that you make.

@Eddycurrent - There's no doubt that polyline 13 IS closed - I have been cursed in the past by 'enclosed' figures not being so.

[dh42]

Hello

With Mach3, you can also use a setting that switch automatically from constant velocity to exact stop depending of the angle to bee cut. It allows you to get the best of both worlds.

In "general settings", have a look on "Stop CV on angle > ..."

https://www.machsupport.com/wp-content/uploads/2013/02/Mach3_CVSettings_v2.pdf

++
David

[JG]

Hello

With Mach3, you can also use a setting that switch automatically from constant velocity to exact stop depending of the angle to bee cut. It allows you to get the best of both worlds.

In "general settings", have a look on "Stop CV on angle > ..."

https://www.machsupport.com/wp-content/uploads/2013/02/Mach3_CVSettings_v2.pdf

++
David

Thanks David, I had understood that from watching the video that was linked to by Pixelmaker.

I have now changed the setting in Mach3 to Exact Stop - I suspect that (for my purposes) it will be the best solution, as I've said, speed is not an issue - and I would sooner have the highest precision.

[dh42]

The better way is to set "Stop CV on angle" in Mach3, but it is better to use Constant Velocity each time it is possible, not only to avoid slow movement but also to avoid the machine to jerk with things like "free" curves or any other toolpath that are done with a bunch of little segments (text/logo engraving, 3D machining, etc)

The Exact Stop / Constant velocity is set in the mop itself. If "Velocity Mode" is set to Exact Stop / Constant velocity, this override the default setting in Mach3 by writing a G61 or G64 at the beginning of the mop . If it is set to "undefined", no G61/64 will be written and Mach3 will use is default setting or the previous setting encountered in the Gcode. (depending of the default setting in your PP, a G61 or G64 is written, or not, at the beginning of the Gcode)

It is a good idea to choose yourself, for each mop, what is the better mode to select. Constant Velocity in mop setting + Stop CV on angle < 90° is a setting that works for almost all jobs.

I have now changed the setting in Mach3 to Exact Stop - I suspect that (for my purposes) it will be the best solution

This is only the default setting that will be used if no other has been defined in the GCode, but if another mode is selected in the Gcode it will override the Mach3 default setting.

Have a look at the beginning of your Gcode, if you find a G64, that means that your PP is set to Constant Velocity by default. If you want that a mop will be cut in exact stop, change the mode in the mop itself.

For my use, I have this settings:
- in The PP > set by default to Constant Velocity
- in the mops, set by default in Constant Velocity too

So, if I need a mop to be cut in exact stop, I just need to switch this mop to exact stop, and do not worry about the others.

++
David

[JG]

Thanks for that update David - a very thorough evaluation of the real situation.

I've now found the [Velocity Mode] setting within CamBam so it does make more sense to leave Mach3 on CV and use that setting when ever I perceive a likely 'issue' with corner rounding.

Now that I've become aware of this 'corner' issue, I can see that some other profiles in my current project have also been affected - as it happens it made very little difference but at least I can now take account 

I read this forum daily and glean a great deal from it though the amount of work I do means that I seldom have need to ask questions, but I'm very grateful that it exists !

[lloydsp]

JG, I'm confused.  I thought you said that the CV issue 'was the solution'.  Do I understand, now, that it did not fix it?

Lloyd

[JG]

JG, I'm confused.  I thought you said that the CV issue 'was the solution'.  Do I understand, now, that it did not fix it?

Lloyd

Appologies for the confusion Lloyd, I have not actually re-cut the job, I've just surmised that the CV issue of 'rounding corners' - except the start & finish of the path - made absolute sense.

For this particular job, there is a second operation to be performed from the opposite side of the work (this needs specificly rounded corners) which will give me access to a 'through hole' and I can then clean these inner rounded corners with a file - I'll even need to do that for the first corner which naturally has a small rounding due to the size of the cutter used (1.5mm) but I do need it to be 'square'.

It may help you to know that the job is a hole in a box for a drawer; the drawer is square (well 20 x 35.5mm) but the front of it is 25 x 45 with 3mm radiused corners.
Better still - see attached image.


Should I find that the [Velocity Mode] setting does not correct the problem (the next time that I find that I have need for such) then I'll certainly report back