Anyone having an issue with carving a circle or hexagon and having uneven thickness of the walls?
I have tried many times checking my files, but the carve still comes out different thickness on the right side as opposed to the left. Any help would be greatly appreciated.
Software I’m using is Aspire 11.5
There are two separate tool paths in my process. I do re-home for each toolpath using the touch probe.
-Pocket using .375 bullnose bit
-Profile using a .25 endmill
After the carve I end up with .27 wall on the right and .19 wall on the left, should be the same. Hope this makes sense.
Try NOT rehoming the X and Y (Do only Z). I suspect you are hitting different points on the bits (i.e. the cutter is wider than the core), or you are not setting the software probe diameter to your .375 diameter vs the .25 diameter it likely defaults to.
I experienced something similar: I saw the non-symmetrical sides issue when carving a circular molding toolpath. Everything looked perfect in VCarve and the other toolpaths (pockets and cutout profile) on the same piece were spot on. Interested in how this topic develops.
Thanks for the input, the pocket seems to carve fine with the .375 bit, I do add that to the probe setting. Once that path is complete I need to switch to the profile bit, which is .25 endmill so I feel I need to re-probe because of the bit change and width etc. I am baffled why this isn’t working properly.
However you have made me think of doing a test with the same bit .25 for both toolpaths just to see if its user error or not.
You need to probe Z only the second time.
How thick is your wall supposed to be? You have a variance of .08, which is between 1/8" and 1/16". Assuming that the cuts are just shifted, your offset is actually .04" at the centre. That would mean your wall is supposed to be 0.23" thick.
An offset of 0.4" is 1/24th of an inch. Assuming some rounding etc, it may be that your offset is really 1/32" (I’m guessing you are going for a .25" thick wall). I’m still thinking that doing the probing and hitting a different high spot on each cutter may be causing this. You may also want to actually measure your cutters to make sure they are the size you are telling the software. Sometimes you get people selling metric bits as imperial sizes, etc. I.e. It’s only close, not right on.
I’m a little confused and that’s because I’m new to this so please bare with me as I really appreciate your help.
So are you saying that even though I going from a .375 bit to a .25 bit I only need to do the Z setting?
You are correct on the wall thickness it should be .2338.
I will measure the cutters since I have not done that.
The purpose of the XY Probing is the find the centre of the bit. Center never changes with bit size. You need to tell it the width of the bit so that it can calculate where the centre would be since you are probing from the outside edge. You may find that with some bits it is better to do a XY setting with a 1/4" end mill, then immediately swap it out and put in the bit you want (e.g a V bit) and do the Z probe.
You should only need to probe XYZ when booting up the system or if something bad has happened (router got stuck, etc.). You definitely need to do Z each time because the amount a bit extends will change every time the bit changes.
Zero XYZ at beginning of cut and only probe Z with each bit change
Thank you Atroz,
I will try this later today and let you know the results. I’m feeling excited, I have spent days trying to figure this out and even though I haven’t tested feel like it all now makes sense, thank you.
Thank you Borgori,
I will be trying this later today!
Thank you so much for your help, that worked great all sides even.