Cutting tabs

[Chips]

Hello eveyone,

This problem just started for me. The Shark was working great.
A very simple project -- 3 inch wheels cut from .5 pine using a .25 end mill
To ready the machine I align the cutter over the pine board where I want the cut to begin and set x, y, and z to zero. The controller is on during this process. Once this is done, I load the .tap file and start the cut. I ‘ve done this many times before without issue.
On this project the Shark is set to the following.
Pass depth is .125
Step over is 0.001
Speed rate is 20 (Tried 40 and 60)
Plunge rate is 15 (Tried 20 and 30)
Tabs set to L .125 W .125
In the attached pictures 1, 2, 3, 4, pic 1 is the most pronounced and is cut on the backside of the wheel looking from the front of the machine. I can work with 2, 3, 4, but 1 is terrible about a 3/32 gouge.
I also attached the Vcarve and .tap files for review.
Is it possible one of the axis is out of alignment ? Would or could that cause my problem.
Any suggestions…

Thanks Chips

[jeb2cav]

Hi Chips,

I haven't been cutting any circles, or shapes this deep. However, you may want to read the VCarve online doc, specifically look at the leads and the ramps seeting for the profile toolpath.

I would guess that picture 1 is where the cutter starts and ends (the worse one). I think you can minimize or remove some of the edge marks on the wheel by using a lead. It may not need to be very long at all. This is on p116 of the online pdf.

For the marks along all 4 tab locations, you may be able to remove or at least minimize that by selecting the "Create 3D tabs". This enables the tab to be created with a much smoother motion - it doesn't plunge up or down at the beginning of the tab (non-3D tab), but move up and down while continuing to move along x and y. From your pics, it looks like that groove is aligned with your tab edges. This is on p114 of the online pdf.

I have a job running, or would go and give this a kick right now. I don't think this is an alignment issue with your shark. It may turn out to be an accuracy capability issue, but we're not to that point yet. From the manual, it seems like these options are available for this toolpath to address what you're finding when not using them.

[Chips]

Hi Joe

Thank you for the info. I haven't read the online doc but I will after this response. I will let you know how it turns out. Again, thank you for the info.

Chips

[Hobbyist1015]

HI Chips,

I'm so glad I am not alone in this matter. I'm also having the same problem you're having with the cnc shark cutting tabs. I hate when it leaves those 2 nasty mill marks in the wood where the tabs are located. I also submitted a forum on here and the link to that is: http://www.cncsharktalk.com/viewtopic.php?f=2&t=597. When you look at my link view the picture I submitted. It's looks exactly the same as yours. Not everyone is having this problem only just a couple people and it seems like were the lucky ones.

I hope we can work together on this matter and get this thing figured out. We spent a lot of money here and this machine needs to work top notch in my opinion. I currently have the techs looking into this issue. They may want me to send my controller in for testing.

Thanks!
Steve

[Hobbyist1015]

Hi Chips,

Please let me know if you found anything out on this matter. Thanks much!!

[Buc]

To All Tab users,
I use Aspire 3, so I maybe be unknowingly posting bad information for V-carve users. This information should work ok with V-carve v6. The order button tab I was an addition to the new version upgrades of Aspire and V-carve.
This is how I set up my tabs. Select profile tool path. Machine vectors, Check outside/right direction and check conventional.
Click on the tabs button check add tabs to tool path. Length = .3". Thickness = .125". Check create 3D tabs. Click edit tabs button, check constant number (4). Check first tab at machining start point.
Skip leads tab - not used.
Click ramps button. Check add ramps to tool paths. Check Spiral.
Click on order button. Check left to right. Check bottom to top. Check grid.
Skip corners button - not used.
Also I use a .125" E.M. instead of the .250" E.M. Sometimes, if I'm not multi-tasking I set my depth of cut .010" to .020" less than my material thickness and leave an onion skin and finish cutting part out with a utility knife and forget the tabs entirely.
Hope this helps and everything I said is clear. Any Questions? If I don't know the answer, I'll make something up....(Joe, draw up some pictures)
Buc ($0.05)

[Chips]

Steve,

I’ve been out of town and not able to work on a cure for our problem. I did try Joe’s suggestion before I left. It did help a little using the 3d tabs, but I still have small groves depending where on the table I cut the circle. For whatever reason the groves are more pronounced in the middle back of the table. I think the table is square and flat because I ran a .5 em over the entire table. I did notice the Z axis has a little play (1/16 movement) front to back which may contribute the problem. This weekend I’m going to break the machine down and check for lose bolts. Will let you know if that helps. Do you have any suggestions or comments?

Chips

[Chips]

Buc,

Thanks for the suggestion. I'll try that before I tear the machine down. As for the onion skin method I'll pass on that. But thanks.

Chips

[jeb2cav]

In addition to Buc's detailed guide, and given your comments about table being square - there is some give, but you would only experience it if the plunge was too agressive for the cutter/material combination. So another thing you can try adding to the equation is lowering the plunge rate to see if this "goes away".

[Buc]

Chips,

It is reccomended to use a down-cut spiral end mill for cutting profiles. For drilling holes and rough milling, use an up-cut end mill. Also my machine has more give than I would like to see. That is the reason I use a smaller diameter end mill for profiles. It doesn't have a tendency to push or allow the cutter to push away, or in your case to push into the part. Just have found to have better luck with the smaller dia. I guess I ran industrial strength machines for way too long. You may want to play with the FRO and RPM's, to find the sweet spot of your machine and your end mill.

Buc