Hi,
I need some advice. I have created a toolpath in meshcam for a part that has a narrow groove on its surface. When I view the toolpath the waterline path in the groove is incomplete and there is a ‘cat’s-cradle’ of unnecessary red rapid-move paths.
The rectangular loop groove is 1.67 mm wide and 1.7 mm deep. The two short straight grooves are 1.67 mm wide and 1mm deep. The 0.063" tool is 1.55 mm in diameter.
Thanks for listening.
As mentioned elsewhere, a good rule of thumb is that MeshCAM “doesn’t see” features that less than ~10% larger than the diameter of the tool.
1.55 mm X 0.10 = 0.155
1.55 mm + 0.155 mm = 1.705 mm
1.67 mm X 0.10 = 0.167
1.67 mm + 0.167 mm = 1.837 mm
I’m concerned that the width of these features are very, very close to this “limitation”.
@Randy has much more experience with MeshCAM than I do so I bet he’ll jump in and have some advise.
Thinking on this more…
mark
Thanks Mark, this helps me understand the problem.
If I create an imaginary tool bit with 1.45 mm diameter and set ‘Stock to Leave’ = 0 then the toolpath shows the expected waterline circuits though the groove. However, I believe if I run this job using the 0.063" (1.55mm) tool the grooves will be 0.1mm wider than the drawing, is that correct?
Since I don’t have a toolbit smaller than the 0.063" tool, is there another way to create a toolpath that the 0.063" tool can cut? Or do I just have to wait until I can get a smaller tool?
Cheers,
James/.
If I create an imaginary tool bit with 1.45 mm diameter and set ‘Stock to Leave’ = 0 then the toolpath shows the expected waterline circuits though the groove. However, I believe if I run this job using the 0.063" (1.55mm) tool the grooves will be 0.1mm wider than the drawing, is that correct?
MeshCAM will honor the feature characteristics - when it can “feel them”. @Randy describes the process as a blind man with a stick (the tool) feeling around. The “feeling around” does the best it can however the math and logic used to do this have limitations. If the features is less than ~10% over the tool diameter the process doesn’t poke the stick into the feature - it’s doesn’t feel/see it.
Since I don’t have a toolbit smaller than the 0.063" tool, is there another way to create a toolpath that the 0.063" tool can cut?
There are two settings that affect the ~10% number. Since you’re “on the edge” these may help. These are things one should be doing anyway.
A) The MeshCAM tolerance setting should be 0.0001" (or the metric equivalent).
Give MeshCAM the ability to work the surface with the finest possible tolerances.
B) When your CAD package spits out the STL file, tell it to output as many triangles as it can.
Give MeshCAM as much data to work with as possible; the best possible approximation of the surface.
If you’ve got a computer with a 64-bit OS, 4 GB or more of memory, and 2 or more high speed cores, let MeshCAM crunch! The more time spent analyzing the STL file, the better the machining.
Or do I just have to wait until I can get a smaller tool?
Trying the above things (and use them from now on) and see what happens. If the setup is just too close to the edge of how MeshCAM works, you’ll need to go smaller.
MeshCAM will use a smaller tool to create a larger feature but applying the necessary operations.
mark
Thanks Mark, this is all useful information.
I will try your suggestions tomorrow.
What is ‘stock to leave’? Is it ok to set it to zero?
Cheers,
James/.
Roughing is the process of attempting to remove the bulk of material that needs to be remove quickly. Finishing is the process of cleaning up what the roughing left and obtaining a nice finish.
Because roughing may go much faster than finishing, the roughing may tear, dent or harm the stock. We want to leave a bit of stock on top of all of our features to ensure we don’t harm the finish - prevent any potential “digging into” the stock such that penetrates to the ideal surface we’re after. The finish pass(es) will take care of what is left.
One of the parameters that goes into the “feeling around” that MeshCAM does is “stock to leave”. One has to leave the stock specified and deal with the fudging MeshCAM has to do and still get the tool in the feature.
Roughing with “stock to leave” at zero? That would usually not be the case - one is trying to go fast - but if the roughing is gentle that OK.
Remember there are multiple passes. Just because the roughing doesn’t get it doesn’t mean that the finishing can’t get to it. When a feature can be machined without roughing depends on the material, the feature, the tool, the desired finish… and so, being complex, we usually try to rough first. With practice, one gains a feeling for how to be OK without roughing for these special cases.
mark
Digging into the picture you posted, the tolerance is way to big. The 0.0001" is 0.0025 mm.
You stock to leave os ~0.5mm. For a groove the stock to leave affects the sides and bottom. Pretty hard to get a 1.55 mm tool into a 1.67 mm wide feature when ~1 mm of it is already spoken for! 
How small to set the “stock to leave” depends, somewhat, on the material you’re machining. For some jobs 0.5 mm is just fine. In others, one can go much smaller. Something in the range of 0.1 to 0.2 mm works for many materials. YMMV.
mark
James, Mark is exactly correct about the need for the tightest calculation tolerance in this case. There is a relevant thread http://grzforum.com/viewtopic.php?f=3&t=15169&p=23062 on the MeshCAM forum, and a search over there of “slot” will yield more similar discussions. As I’ve said over there, my own rule of thumb is to use a cutter 90% or smaller of the given hole or slot size. And I always use .0001" (.0025mm) calculation tolerance on all my final toolpaths.
Randy
Hi Mark and Randy,
Thanks for your comments which have helped me to understand why a slot can’t be cut with a tool close in size to the width of the slot. It makes sense now.
I tried 0.0001 tolerance and disabled the roughing cut. With that it found more of the slots but it’s doing some funky wiggles along the path.
So I’m going to wait and get a smaller tool and do it properly.
Thanks again 
James/.
The other option would be to get a different CAM application for this task. G-wizard editor has a “conversational CNC” program that can do simple slotting moves like this with relative ease, and lots of videos and tutorials to help you understand how to use it, which can be a bit tricky, since it’s aimed at more experienced CNC people. And I’m sure Fusion CAM and a host of others could do it pretty easily.
I really like MeshCAM, it’s great for what it’s meant for, but it doesn’t seem, at least to a novice like me, like it’s always the best choice for every operation.
To that point, can anyone recommend a really solid 2.5d CAM package that doesn’t cost a ton and is relatively approachable? Does that even exist?
I hear that there is this program - Carbide Create - that might be the 2.5D program you are looking for @MrHume Would live to get my hands on it also 
Thanks for making me aware of these other options Mr Hume.
The Vectric packages VCarvePro and Cut2D (both 2/2.5D programs) are immediately available choices. There are Nomad post processors for them by one of the members of this forum.
mark
