Two-sided cutting is "off"

[pknvectric]

I created the two identical vectors because I wanted to profile cut a shallow v-bit around the exterior of my cabinets (just to knock the sharp edges down before cutting the parts out with a 3/8" compression bit.)

Using a profile tool path .05" deep and the 90 degree tool is OUTSIDE w/ an Allowance Offset of -0.0231. It works perfectly on "Side A" but when I flip it over and run this on the backside it's off a little. The X-axis moves are exactly correct. The Y-axis are off. (The tool cuts properly (just outside the vector) as it moves horizontally on all of the X-axis cutting but on the Y-axis it's off by 3mm-ish.

Why isn't it cutting exactly where I expect?? (Yes, my sheet should be properly aligned on Side B. My CNC has pins so the sheets is in an almost identical position after flipping it over.)

[TReischl]

The very first thing I do when something like that happens is take a look at the gcode. In this case I would take a look at the Y values on both sides. If they are the same it means you are dealing with a job setup issue or a machine issue.

I would also double check that the two sides are properly positioned in the software. If they are you can bet that the post has not mysteriously moved them.

[IslaWW]

Are you doing a sheet trim prior to the flip? Variations in dimension or being slightly out of square can cause this.

[garylmast]

I had a similar problem, that it turned out that my alignment lines that I marked on the spoilboard was not parallel with the X or Y Axis, causing my material not to be square when I set it up. Once I corrected that, the problem was solved.

Gary

[pknvectric]

No, the material isn't being trimmed / altered in any way prior to flipping.

In effort to prove that I was doing something wrong I changed tools, used a different offset & depth but the problem was identical.

Next I created a new rectangle and bumped it left 2mm. Problem solved. I don't like a jury-rigged solution like this but it solved my problem for the time being. The only cutting I'm doing on the bottom side of the sheet is not mission critical as far as the X location of cuts (I.e. 5mm shelf holes and pocket holes) so it makes me wonder if everything on the Bottom of the sheet is off 2mm. I don't think this is the case but something weird is happening.

I'm out of the office this week so I won't be able to test this theory for a while... (I suppose the best way to test this would be to cut a 10mm hole 3/4 of the way through the sheet and then flip it and see if they line up exactly. Other / better suggestions?).

A few weeks ago I machined both sides of a piece of 12mm Baltic Birch (using fixed set screws in my spoilboard to verify it was flipped exactly correctly) and if I remember correctly it was still off a bit (but not much - certainly less than 2mm.). More feedback to come when I can test the Baltic birch again...

Overall opinion on Vectric's two-sided machining? Thumbs up. It is fantastic / powerful.

[Wayne Locke]

Measure the material. It is probably not exactly as expected. As Gary said do trim cut.

[rscrawford]

I might be wrong, but it sounds like you are using your machines pop up pins to place the sheet for two sided machining?

In this case, if the sheet size is off by .01", your two sided cuts will be off by double that, or .02" when it is flipped. (you are referencing from different edges of the sheet when you flip it).

If you are drilling index holes and your two sides do not line up, then either your gantry is out of square or your spindle isn't perfectly trammed.

It is not a problem with the software, its a problem with your machine or set up.

[TReischl]

Like I posted earlier: Check the gcode! That is the final word in where your problem lies. If both the programs have the same X and Y maximums then the problem lies somewhere on the machine. Axis out of square, etc.

I know it is easy to think that somewhere, deep in the bowels of the software, a gremlin is moving things around. That is extremely RARE. Think about it, this software is used to literally create billions of lines of gcode everyday. If there were a gremlin there would be lots of posts.

If you have another software program that is capable of reading eps, dxf, ai etc a way to see what is going on is to export those vectors and see if they match up like they are supposed to. If they match up then it is time to start looking seriously at the machine. I have no idea how the Camaster machines home/zero their axis. Some machines use one limit switch, others use two. On the machines with two switches (usually precision micro switches) those switches not only home the axis but also square it. So if those two switches are not in the proper place it will automatically square up the machine out of square. On a single switch machine like mine I have two solid stops that I position the axis to with power off. Then I power up, move off the stops and then home on the single switch.

A really qood way to check squareness of X to Y is to get a piece of mdf (I use 1/4 inch). Machine a reference edge that is screwed to the spoil board in line with the base axis of the machine. Then mill two slots,(the ones that are farthest apart) flip, move over a bit and mill the same two slots. Make sure you reference the same edge when flipping. Then compare the distances between the pairs. Whatever the difference is amounts to twice the error. Here is a pic to help with all that verbiage:

The more distance you can put between those slot pairs the more accurate your squaring will be. IMHO squaring a cnc machine with a "square" is a fool's errand.