MeshCAM and Carbide Motion Workflow

(Temujin Kuechle) #4

I finally had a break from work to come back to the issue of surfacing the spoil board.

The whole process seems to start off correctly, but then it doesn’t start milling from the center.
At a certain point, after air cutting almost a square, there is a limit switch error.
I tried the setup a 2nd time, but now I have a step in my spoil board and it is also off set.
At the moment the Nomad is cutting that second step, but I also noticed that there is a small protrusion where the Nomad seems to have skipped out on milling altogether.
Why is it offsetting from the left edge about 1 5/8" and about 1/38" from the front edge?

0 Likes

#5

@Tem, there is not a “correct” place to set zero in MeshCAM. You can set it most anywhere you want. The important thing is to set the same zero in Carbide Motion during your setup.

If you have set your Program Zero in MeshCAM to the top center of the stock, when you set up the run in Carbide Motion you will move the cutter to the center of the stock and down to touch the surface of the stock. Then you need to zero the Carbide Motion coordinates at that point

That is the step that some folks have forgotten to do. Without zeroing the coordinates where the cutter actually is, Carbide Motion will cut the gcode from wherever the zero point happens to be.

Carbide Motion is a numbers-driven program, so coordinating MeshCAM’s Program Zero and the zero point in Carbide Motion is the key to physically cutting in the right place.

(Reading back, this is just exactly what @UnionNine said earlier but it is a fundamental point)

0 Likes

(Temujin Kuechle) #6

Hi Randy,
Thank you for the advice.
I followed the wrench tutorial process.
But still had the offset X & Y issue.
In MeshCAM I make sure to zero all to the Top Front Left Corner. This is the same location that I zero the cutter in CM.
When I run the NOMAD, CM centers the cutter in a location offset from center. That is what I am not understanding.
Should I zero all first, then move the cutter to the TOP FRONT LEFT CORNER?
In MeshCAM, the origin axis thingy seems to be at that location too, so I think I am setting 0 properly.

0 Likes

#7

How have you defined your stock in Meshcam? Have you set the size to 8" x 8" by 0.5"? I’m asking because from the photo it looks like you may have defined the stock incorrectly - so carbide motion thinks the stock is a different size.

And what size cutter are you using? I can whip up a gcode file that you can load into CM which should, if you zero to the bottom left of the waste board, cut just fine.

And in terms of zeroing in CM - are you moving the cutter to the front left, clicking set zero, then clicking on zero all? At that point all of the values should read zero. So wherever your cutter is at that time, CM will read as zero. I feel like perhaps you are clicking on set zero, but not then clicking on Zero All.

0 Likes

#8

@Tem, your screenshot shows your MeshCAM Program Zero at the front left bottom of the rawstock. Is that what you intend? If the Program Zero were at the top of the rawstock, the green and red axis lines would be at the top.

From your annotated photo, you are setting the Program Zero at the top left front of the sacrificial board. If you are machining the whole spoilboard, that is not in keeping with where you have the Program Zero set in MeshCAM

The toolpath will generally not start at the Program Zero. The roughing toolpath will generally start near the center of your rawstock and work its way outward. So the start of your machining is not unexpected if you are machining the whole spoilboard (facing it to a level surface, for example).

It would help to understand, if you attached a screenshot of your job in MeshCAM.

0 Likes

#9

Okay - here is my workflow that I think is simple enough to follow :smile: It may not be the best way to do things, but it worked well for me.

Step 1: Import an image of a black square and set the size to 8" x 8" x whatever (I’m not sure this matters since we will be changing it shortly, but I set mine to .35") Also check “Black is Z+”

This is what you should see

Step 2: Set the stock size - this is the size of your wasteboard. Set it to 8" x 8" x .35" (although the Z height isn’t as important since we are going to set the max cut depth shortly). Click “Lock stock dimensions”. Also set the Z to zero, so the image is at the top of the stock

This is what it should look like now

Step 3: Set the max cut depth - this is the amount of material you will be cutting off of your spoil board. I have set this to .02" and it has worked well for me

Step 4: Make sure your zero is set in the right place, as shown in the pic

Step 5: Set your machining parameters. Here you don’t want a roughing pass or anything else - just “Cut along X.” You don’t want to set the machining margin too large or else you could hit the tool probe - I have used 1/2 of the cutter diameter in this case. The feed of 40ipm should be fine, and the depth per cut of 10 is fine too. I think a stopover of 1/2 the cutter diameter (in this case .0625) is fine.

This is what the path looks like

From here, all you need to do is make sure you zero the machine properly. I have a way of doing this that’s not so easy to write about - I think I’ll need to shoot a tutorial video soon :smile:

0 Likes

(Temujin Kuechle) #10

About the zeroing process:
Do I zero out xyz in CM before jogging to the 0 location for xyz on the stock and setting the 0,0,0? Or just locate 0,0,0 on the stock and zero xyz, because thats what I had thought was the process.
By the way, I was not able to move the Z0 location in MeshCAM for some reason.
I was obviously able to crete a job in Mesh CAM but am not able to retrieve the tool paths, aside form an .NC file. I will not be able to access MeshCAM for a a few weeks.

0 Likes

#11

In CM, move the cutter to where the 0,0,0 position is and then zero XYZ at that point.

If you are working from an STL input or extruded DXF in MeshCAM, you can set the zero point with the Set Program Zero command in the CAM menu.

If you are using MeshCAM 6 and working from a bitmap input, you cannot move the Z0. That is a bug in V6. In CM, instead of zeroing Z when the cutter is touching the stock, you will need to type in the Z value corresponding to the stock top surface from MeshCAM (if your geometry is .100" thick, the top of stock is Z+0.100 and so on)

0 Likes

(Temujin Kuechle) #12

Thanks Randy. So, I am fairly certain that I am doing all these steps in the right order.
Would having the Z0 located below the stock contribute to the offset issue at am seeing when attempting to surface the spoil board?
The problem is the cutter going all the way to the right side and hitting the limit switch.
Cheers!
Tem

0 Likes

#13

Z0 difference wouldn’t have anything to do with X and Y. One thing to check is whether the units–mm or inch–are consistent through the workflow. One problem some people have experienced was that they didn’t notice MeshCAM was importing the geometry as mm with them thinking it had been inches. 20mm and 20 inches make quite a difference! :slight_smile: Could you zip and attach your gcode? You said you don’t have access to the MeshCAM machine for a while but the actual gcode will give a good clue as to what is really happening.

0 Likes

(Temujin Kuechle) #14

Yes, I’m away from my workstation that has MeshCAM. On vacation actually until mid August.

0 Likes

(Temujin Kuechle) #15

Hi Guys, It still begins cutting about 3/4"positive X from center and 3/4" negative of Y from center. Z is as expected. Why would there be a 0.75" offset in X and Y to begin cutting when the tollbooth preview in MC shows a very centered start location on the stock?
I’ve completed all the steps in order in both ways suggested to me.
Still a huge offset is causing the issue repeatedly.
Thanks.
Tem

0 Likes

(Temujin Kuechle) #16

Finally, an inkling of progress. If I am understanding correctly, the XY center was referencing a slightly oversized spoliboard STL file (9"x9", late night visual delusions? Funny, I never went back to check those DIMs). It seems like this caused the .75" offset.
I also set just an X pass, no roughing. I increased the federate from 5 to 10, so I am getting more chips than curlies. Its humming a bit more, but not like my first try, when I didn’t have one of my wifes old foam sheet yoga matts under it.

0 Likes

(Temujin Kuechle) #17

Some progress on cheap 12mm thick sheet of HDPE.
It got loose during the last few minutes. I had just used double sided tape, next time maybe something more substantial is news for work holding. The vise might be too small for this size project (145mmx160mm), I don’t know. Regardless I need a 1/8" ball end cutter (I got 2 squares and one was mislabeled on the kick starter delivery). I need to order a bunch of stuff anyway from the store so I’ll be ordering 1-2 more of those any way. I’m just starting to get the hang of how this works. I’m really enjoying the learning aspect. By the way, how do I stop plastic from building up a big wispy mass around the cutter? Thanks!

0 Likes

#18

HDPE is a low-surface-energy plastic, similar to Teflon and Delrin, adhesives don’t stick to it very well. So yes, screwing it down to the spoilboard would help a lot.

The closest I’ve come to machining HDPE is Delrin (acetal) but there is some discussion on the Shapeoko board at http://www.shapeoko.com/forum/viewtopic.php?f=7&t=3808 The numbers might be agressive for the Nomad, but the message seems to be keep the feed rate up and adjust the depth of cut to not bog down the spindle.

That’s a neat looking workpiece. Is it a surfboard fin?

0 Likes

(Temujin Kuechle) #19

Hi Randy, yes it’s a type of surfboard fin that fits into a slotted box. the ability to remove the fin for traveling on airplanes is great because they don’t get knocked off or forced theough the fiberglass shell, which leaves the board basically very limited or worthless.
I’ll try pre-drilling the sheet outside of the area to be milled and then use some screws to fasten the sheet to the spoil board. Using the Nomad set-up feature seemed to work very well. Thanks for the speed and feed link, I’ll review it soon.

0 Likes

#20

I had great success with King Starboard (got it at TAP Plastics), a really nicely machining HDPE plastic - only perfect little comma shaped chips, no strands or hairs or melting at all so I never had an issue with stuff stuck to the cutter. FWIW I was able to machine a lot of it quite successfully with just sticky tape, even when trying to stick the bumpy side down. It didn’t stick as well as it did to wood, but it would have certainly worked for that fin you were trying to cut out if you put tape all over the bottom surface. Thought since you’ll need to screw down the piece for the second side, you might as well just drill the holes and screw it down to fasten it.

0 Likes

(Temujin Kuechle) #21

kjl, thanks for the resource link. TAP is kinda not too convenient for me. I go to the local store, Gary’s Plastic Place, in Santa Cruz.

0 Likes

#22

You can order from TAP online if you want. If not, Seaboard seemed to be basically identical to Starboard except not quite as good with the sticky tape but still good enough for milling…

0 Likes

(Warren Bailey) #23

I do a lot of HDPE and exclusively use Nitto tape (Permacel P-02). Sticks great, but good to not leave it for a week like I did with one piece - challenging to remove. Also, had some “stranding/birdsnest” issues and upped the feedrate and this went away.

0 Likes