Inaccurate cuts

[Anonymous]

Hello All,

Fusion 360 is an outstanding program. However i am having a problem getting exact cuts. Every cut is off by .1 to .07 of an inch. I have a X-carve, using UGS and GRBL. The X-carve works fine if I use Easel (Inventables X-carve cad and cam program). However Easel does not have the functionality of Fusion 360.I have turned off stock to leave, played with tool diameter. Any ideas would be a great help. Thanks

[Anonymous]

Can you post an example progran that does function correctly in X-Carve? My guess is that you either have mechanical issues and perhaps have been lucky when using Easel, or you need to get a post processor that X-Carve understands. Think about it logically:

1) Easel is meant to work with X-Carve, and has been optimized to produce toolpaths that X-Carve understands.

2) Fusion produces code that works fine on machines with 100 times the precision of X-Carve, so it is 100% impossible for Fusion to be generating toolpaths off by .1-.07 inches.

3) Fusion is using the same math to calculate toolpaths for every application, which occurs prior to post processing.

4) There is no optimized post processor available (that I can tell) for X-Carve.

If those facts are true (I'm positive about all but number 4), then the problem is one of three things.

1) User error when programming in Fusion (not likely, but a posibility that something like the tolerance setting is set to .1" instead of .001")

2) The post processor is not correct for the machine.

3) The X-Carve is not mechanically sound. 

My experience with users that have light duty machines is that the problem usually resides in the mechanical end of the spectrum. Maybe it works fine with Easel because it is not asking too much of the machine, where you may be setting your feeds/speeds in excess of what the X-Carve can actually handle. Maybe the times you have used Easel were under different conditions from those you tried using G-code from Fusion (Noise from something in the room causing stepping problems, etc.). Maybe a set screw has loosened and you are getting some backlash. 

If it were me, I'd comb through the machine assembly and be sure everything is right and tight. I'd then be sure that the programming in Fusion is apples to apples in terms of feeds and depth per cut, while also using a post processor optimized for your application. If you are still having trouble, I'd then go back and send some hand written g-code with test shapes to determine if there is a problem with how the g-code is being processed. If I understand right, Easel connects to the machine directly, but G-Code must be sent through a different application that works as a translator. If that's true, the main difference between using Easel and G-code really comes down to that translator. Assuming all the mecahnical stuff is right, and knowing that Fusion outputs perfectly accurate code, the translator seems to be the spot where there is the most unknown and where I would be most suspicious the problem is stemming from. It may need a very specific g-code to work right, including how many decimal places the code contains before it may actually start rounding numbers.

[scottmoyse]

---

@Anonymous wrote:

4) There is no optimized post processor available (that I can tell) for X-Carve. 

---

The grbl post that ships with Fusion works perfectly well with Shapeoko 2 & X-Carve. 

[Anonymous]

Hello all,

Thanks to your suggestions I have taken the following steps:

1)Checked tuning on X-carve-Comes out exact every time.

2)Tried to carve different size squares and circles. From .5 up to 5. The larger the cut the greater the  amount of error.

3) Tried different G-code senders and different post processors and all the cuts had the exact amount of error for the given size.

4)I have cut the same size multiple times and get the same amount of error for all cuts.

All this being said I feel like I have something not set correctly or a setting that needs to be adjusted.I can fudge the size of the part and get a cut exactly what I need however this is time consuming and aggravating. So far all i am cutting are test squares and circle pockets. Any other parts I have cut have also been off. Being new to the world of cad and cam any ideas would be greatly appreciated.

[Anonymous]

Based on that information, my thought is that there is something incorrect about the G-code translator being used in place of Easel. Does USG/GRBL produce the step/dir signal before the hardware controller (in the computer itself) or does the hardware controller get told a motion and it generates the pulse on it's own?

If the computer is generating the pulse signal for step/dir, it would seem to me that Easel is generating the correct pulses, but USG/GRBL combination is not.

Are these two different applications (Easel and USG/GRBL) working off of the same configuration or do you have to configure the controller in each application independently? Maybe the steps/distance setting is correct in Easel, but incorrect in USG/GRBL? That would be my best guess, but I'm not a user of those products and have limited knowledge of what options they have specifically.

Just some thoughts out loud, but I'd need to know more about how that system works to really help much more. In my opinion, you have narrowed it down specifically to the difference between Easel and USG/GRBL since the code works the same (if incorrectly) in USG/GRBL regardless of where you generated it. The G-code is not at fault, the mechanical operation is not at fault, so that leaves only the link between the two, USG/GRBL.

[Steinwerks]

What size are the cutters you're using and what sort of cutter compensation is being utilized in Fusion? .07"-.1" off suggests In Control compensation and 1/4"-3/16" cutters.

If you can, please share an exported .f3d file, the .NC file, and the post processor used. It can be a dummy file, but see if you can make sure the part is incorrect at the machine.

[scottmoyse]

---

@atomkinder67 wrote:
What size are the cutters you're using and what sort of cutter compensation is being utilized in Fusion? .07"-.1" off suggests In Control compensation and 1/4"-3/16" cutters.

If you can, please share an exported .f3d file, the .NC file, and the post processor used. It can be a dummy file, but see if you can make sure the part is incorrect at the machine.

---

Agreed

[Steinwerks]

Whoops, should've been 1/8-3/16".

That's what I get for posting from my phone.

[Anonymous]

Hello, I am using an 1/8" bit.

The following measurements came from the actual cuts from the files I am sending you.

Square:

.5"= 0.4850

2" = 1.9825

5" = 4.9845

Circle

.5" = 0.4765

2" = 1.9745

5" = 4.9870

I used the "GRBL.CPS" Generic GRBL

Thany you for your time and help as this is really frustrating. 

[Anonymous]

---

@Anonymous wrote:

Hello, I am using an 1/8" bit.

The following measurements came from the actual cuts from the files I am sending you.

Square:

.5"= 0.4850

2" = 1.9825

5" = 4.9845

Circle

.5" = 0.4765

2" = 1.9745

5" = 4.9870

I used the "GRBL.CPS" Generic GRBL

Thany you for your time and help as this is really frustrating. 

---

The programming in the F3D file is set to climb mill the pockets. Have you tried conventional milling them to see if there is a difference? How did they get cut in Easel (climb or conventional?). In my experience, a pocket will be a little undersized when climb milling and a little oversized when conventional milling, particularly if you are dealing with a bit in that 1/8" size range. If they are not both climb milling, that may be a reason for a discrepancy. 

I'm going to guess that the accuracy of the calipers you are using isn't really down to the .0005", plus you are probably dealing with wood, so if you round it off the you get somewhere around a consistent .015" in my opinion. Split that in half because half of the problem will be on one side of the pocket and half on the other, so you're talking about .008" or less undersized all the way around the perimeter. You have the tolerance set to .004", so it is only working .004" beyond your permitted tolerance. That's a fair amount more than you'd like to see for sure, but if the bit isn't great (not razor sharp) then I could see that amount being caused by deflection very easily with a 1/8" bit given a nearly full width cut.

The circles will be different from the squares and different from each other more significantly because the attack angle of the bit is not the same as a straight line and not the same as each other since the arcs are varying. Note that the largest circle has the closest deviation as compared to a straight lines (squares) coming in at around .013" off. If part of the problem is deflection due to climb milling, one could expect that the smaller the circle gets, the greater the deflection will probably be if the stepover is consistent. If you're turning into the material with the same stepover, you are likely increasing the effective amount of material the bit encounters, which can cause greater deflection. 

I can't say for sure that your problem is in deflection, but I do think it's worth testing both directions to compare. Also, the quality of the tool has a very significant impact when you're dealing with a small bit like a 1/8" diamter. I would suggest that you tighten up the tolerances to .001" in the toolpath strategy, just to be sure you aren't getting some of it from there. Change your maximum stepover to at most .062 (it's close to a full width stepover right now), but also change your maximum stepdown to around .090 so you are using more of the cutting edge. You can cut about 50% of the width of the tool (max) and about the same depth as the tool diameter (max) with a tool that small in wood. I would also suggest you add in a finish pass and let it be whatever Fusion automatically populates it as for now. Try that out and see what you get. Both climb milling and conventional milling should give you the same results +/- the capability of the machine, but you have to stay within what the tool without deflecting.

[Steinwerks]

I will say I mostly agree with michaelmoe, and want to add that using a Finish Pass is highly recommended to help eliminate issues such as cutter deflection and undersized grinds (most end mills are +0/-.002" for grinding tolerances, for instance).

[HughesTooling]

First a note on the tolerance, with 2d ops the tolerance will only effect splines, lines and arcs with be accurate. Here's a back plot that shows the 2" circle is correct. The radius is 0.9375 * 2 + 0.125 = 2. So there's no problem with the code! I think Micheal is correct and when you use the other program it's not climb milling so the tool will pull into the job not push away. Also if you're machining wood I've read you should be conventional milling.

Mark.

[scottmoyse]

Not true. You have to climb mill with solid timber to prevent grain tear out. Sometimes with soft ply's conventional milling is better. But 80% of the time it's best to climb mill..... BUT

On a floppy machine you may get much better results with conventional milling, simply because climb milling is too hard for it and chatter will set in.

[Anonymous · Accepted solution]

Hi everyone,

Sorry for the delay but works been hectic.

I have finally had a chance to try all the suggestions and am happy to say it was the "mill climbing vs conventional". You guys were spot on. Thanks for all your help.

[Anonymous]

What program are you using to get those descriptions of the gCode operations?

[burkeda]

---

@Anonymous wrote:

Hi everyone,

Sorry for the delay but works been hectic.

I have finally had a chance to try all the suggestions and am happy to say it was the "mill climbing vs conventional". You guys were spot on. Thanks for all your help.

---

Hi, im experiencing the same thing here.  Xcarve, 1/8 bit, etc.  I do not understand the solution here.  Can you kindly describe your fixes?  Much appreciated.  

[burkeda]

Just to clarify my question ... was changing to conventional milling the only thing out of all the suggestions that seemed to make an impact?

[seth.madore]

@burkeda could you start a new thread detailing your issue and supplying the following info:
1) Fusion file. File > Export > Save to local folder. Attach file to the thread

2) Post processor that you are using.

3) Complete description of the problem

4) Pictures if needed.