G-Code Help

[RobieMo]

I am looking for a little help on this one. I am making some Mancala boards and have a bunch of ovals. For some reason there is a small "hiccup" on the ends of the ovals. I have a few guesses why but it doesn't matter. My question is how do you get rid of them? I think I see them in the G-Codes, but then what? I have ZERO experience working with them.

If someone is bored and wants to take a look at it, I would certainly appreciate it.

Thanks,
Rob

[jeb2cav]

Hi Rob,

Can you please post the VCarve project - or at least enough that has the oval vectors and the toolpath set that you are using?

[thepuchman]

I would be willing to look at it but I need more than the code. I can program in code fine but without a print I am recreating your work. I did look at the TAP file and it was all in G00 rapid and G01 linear moves. I did not see any G02 cockwise arcs or G03 counterclockwise arcs. Send me what you can to my email address rnash@vinu.edu and I will look further.

[Buc]

Rob,

Did you try post processor "CNCSHARK-USB_NewArcs_inch"? That will give you the G02 and G03 codes in your tap file. I assume you are using "inch" and not metric.

Buc

[RobieMo]

You guys are the best. Here is the project. To explain a little better, when I run the 3/4" ballnose bit, it makes a pass in a perfect oval shape. Then it moves towards the ends of the oval and adds a couple of points of detail (that I don't want) making the oval not so oval. After that, the bit moves down to the next level and does the same thing. End result is ovals with crooked edges, if that makes sense.

Thanks again for your help.

Rob

[Eagle55]

Any chance of posting a pic of the hicup? The crv file didn't appear to have that. Not sure that it is a problem with the code or maybe something mechanical??

Roger

[jeb2cav]

Hi Rob,

Thanks for attaching the project. I see now what is happening and I think I know why. You are using a Pocket Toolpath - which is fine if that's what you want - and as part of that a large area clearance tool. Most importantly though, it is a pocket toolpath. It is calculating the optimum toolpath to clear a pocket out of the material. So, the two dimples after you run the 3/4" BN as the first part of the pocket clearing you set up, it does 'come back' after going around the oval outline, and cut a bit of the remaining 'inside the oval piece' off.

After Pocket Pass

When you run the clearance part of this pocket toolpath you created - the inside of the oval is completely flat (as you'd expect). The little dimples that were cut as part of the 3/4" BN toolpath were just 'the best way' VCarve found to do this using the 2 tools.

Oval After Large Area Clearance

If you want to carve out the oval, but leave the remaining inside piece, try using a profile toolpath. Here's a pic using a profile toolpath with machine vectors set to inside, and cut depth set to 0.6 (same as your pocket).

Oval Profile Toolpath

Does this outcome now make sense to you? I don't think this is an 'error' in VCarve and resulting tap file.

[RobieMo]

What you said does make sense however I do want the pocket cut out. I am running the 1/4" straight bit first for the clearance run. This seems to be OK. Then I am running the 3/4" BN bit for the detail and finish. This is where the problem is. Hopefully you can see what is happening. The bit makes a perfect oval then moves out to the edge and makes a small detail cut. Following that it moves to the other end of the oval and does the same thing. It is almost like there are some extra lines that got picked up somewhere???

Hopefully you can see the edges that I am talking about.

Thanks again for the help.
Rob

[jeb2cav]

Hi Rob,

In your picture, I see it happening in the center right one - but not the top and bottom right ones. And I see it on the right side of the oval, but not on 'both' sides. It may just be the picture of course.

I'm also a little curious as to the 3/4" cutter you're using. Is this a router bit or an end mill that you has a smaller than 3/4" shank?

I don't see this anomaly in the preview, and suspect it is not in the resulting g-code - but of course it could be.

I did try the project without using a large area clearance tool, with the 3/4 BN, and set the stepover to 2%. Result was a very smooth appearing bottom of the dishes and the same amount of machining time predicted.

One thing you can try that might clear this up is to generate a separate toolpath for each oval. Do one for example on a test piece, and if you don't get the 'small detail cut' - try creating a separate toolpath for each of them. Then when you create the tap file, select them all - you still end up with one toolpath. I have run into this every now and then and in those cases - which I did not take the time to get with Vectric or NWA support on to see 'why' - it did clear up the condition of unexpected toolpath outcome. Not sure it will cure this of course (sorry).

I do look forward to clarification on whether you see this in every oval, or just one/some.

[Eagle55]

I'm kinda with Joe that I'm not at all sure that the problem is the code. I don't have that tool in my data base so it uses some kind of defaults for plunge and feed rates. What I am concerned about is that in the photo, yes I see the problem that you are talking about but I also notice on the left side of that same oval there was an imperfect oval shape. What is the feed rate, the pass depth and plunge rate. I am thinking there might be something to do with these items. Using the programs default settings for a tool not in the database, it appeared to be making 5 passes to cut .6" deep. That is removing a lot of material and depending on the feed rate, may be putting a lot of stress on the gantry. I think I see indications of the gantry flexing (indicated on the left hand side of the oval and a big indication on the "hick up" that you speak of. With that large of bit I think taking about .050 per pass at 30-40 ipm feed rate would be a lot. The proof of this theory is to reduce the pass depth and slow the feed rate down and see what happens.

Roger