tolerance and tight fit design

[supernetdude]

Have made lots of things with Fusion so far, but I always have to make adjustments and play with dimensions to get them to fit together. With this, I don't understand how to calculate adjustments for tolerance. 

In the attached drawing, I have a 9" x 13" panel inset into another body. When I cnc the panel part, it cuts exactly at 9" x 13" outside dimensions. The inset area when cut measures 8 7/8" x 12 7/8". Outside cuts are always spot on, inside cuts are always too small. 

How to I calculate what to change? What would I look at to determine to either add 1/8" to the inset dimension or reduce 1/8" from panel dimension? 

[LibertyMachine]

By rights, they should be fairly close in size to each other, as I don't see anything jumping out at me that would cause this. What control/machine are you using?

One suggestion; You are pocketing out the inside feature and calling it good. It might benefit you to have an extra contour pass come around and take a spring cut. If your control supports it, I strongly suggest using cutter compensation

[supernetdude]

Thanks for the reply. I'm using a CNC Router Parts Pro 6x10. 

I'm not sure what a spring cut is or cutter compensation. I only started with Fusion and CNC last September. 

Thanks for the help. 

[LibertyMachine]

A "spring cut" is typically used to account for any tool or material deflection. Cutter Comp is used to control the size of a part. We program to "perfect size" tooling, but what happens when that tool isn't available, or it's slightly smaller? Cutter Compensation.

What is the Controller, Mach 3, LinuxCNC, GRBL?

Are you using the exact same tool for both operations?

[supernetdude]

I looked up spring cut and found I have to enable "Finishing Passes" which I don't usually do. I have mostly been doing wood and plastic projects and didn't see it as necessary. But still doesn't make sense to me what the inner cut is too small but outside cut is perfect. But I will try the finishing pass settings and see what difference it makes. 

[supernetdude]

I'm using Mach3 with ether smooth stepper, all electronics from cncrouterparts. Same exact tool for both operations, basic 1/4" 2 flute flat bit.

It is still weird to me that anything that cuts that has two edges facing each other is smaller than designed and anything that has edges away from each other is perfect. For example, I cut a cabinet top that has a hinged door in it. The door is 43" wide, the total top is 63" wide. The door has common edge with top. I created single CAM 2d contour op to cut top out, then out of separate sheet of plywood cut the door. The top's outside dimensions are perfect at 63" wide, but the opening for the door was 42.8" or so. The door was perfectly 43".

[supernetdude]

Still looking for help on this.

[LibertyMachine]

With your original .f3d file, there was nothing in there that would indicate any such issue being present. That leaves machine/control or code. What are you using for a post processor?

Could you attach the offending NC code in your next reply? It will need to be saved as a .txt or .nc file format

@daniel_lyall, you know a great deal about Mach3, what do you think is going on? It sounds like he's possibly dealing with a cutter comp issue, but it's weird that it's only presenting on the inside cuts

[Stuart-H]

Seth

could it be the direction of the red arrow ,possible that the inside is being cut on the outside not the inside,

hope PE that makes sense outside cutter is on the outside inside the cutter should be in side

just a guess from a complete I D Ten T as we used to say in IT 

stuart

[daniel_lyall]

There are a number of things that could cause this.

Machine being out of squire, To test for this you just put a pencil in the collet and draw a 3,4,5 squire If the start and end points dont meat it's out of squire.

The ghost offset bug, What is just type G40 and G49 into the mdi to clear it.

The steps per being wrong, What's just measuring the axis movement if you tall it to move 8 inches does it move 8 inches.

Mach3 crapped out, A reinstall fixes this.

RF and EMF interferences, from the VFD, dust extractor (also includes static) or a outside sources. To test for this have the machine off, put a FM radio on the machine tune it into a radio chanell, then turn the machine on, if the radio goes all staticy, you have a RF or EMF leak.

To test for static put your hand on the machine's frame when it's cutting then go touch a bear hunk of metal or a person if you or the person get a zap , you have a static problem.

That's all the simple stuff, what takes minutes to check for if you do one at a time.

The acc or velocity being to high.

This is a Hard one that is easier to test with just the X motor turned on, you can just turn Y, Z and Y slave motor of in ports and pins.

Then run a engrave toolpath with about 20 letters if the start point and end point are the same the X axis is tuned fine, if they are not that's where the problem is if you have ticked off everything else.

Doing this test Mach3 has to do a lot of small moves and this is where Mach3 can fail, if it fails the acc or velocity needs tuned, if not it's something else like fusion being a ****.

Also you can just test once if it's going to fail it will on one run.

@supernetdude post a Gcode that has failed on the machine, You have posted your model so a comprar can be done on the G code in sim, then if I have time tomorrow I could test it on the big machine, what I have dialed in to 0.002 +/- .0001 per 1000 moves per axis.

[Anonymous]

Simple enough to diagnose:

Make a simple design, line two concentric circles or squares.  

Make the cuts, and verify that the problem is present.

Examine the G-code, and check the dimensions.

If the G-code is right, then it's a problem with the machine.  If the G-code is wrong, then there is something to discuss further here.  

I'm going to go out on a limb and bet the machine is wonky.  Backlash can easily account for this behavior.

Try cutting the same part as above, but switch from conventional to climb milling ir vice- versa.  In an ideal world, and on a reasonably good machine this will make almost no difference in the part dimension.  On a machine with mechanical problems, it can make a huge difference, and help highlight the problem.

Regards,

Ray L.

[jasshrie]

I've been having the same issues with my CNC3D kit machine (GRBL) and the gcode looks correct.

I'm guessing that spring or backlash is likely the issue as it only happens on inside cuts and is typically out by about 0.3-0.5mm. I did notice that my machine has a bit more flex in one direction than the other and started nesting the parts with pockets accordingly, but it is a super annoying issue as it will still be out in one direction causing lots of post work on the parts. I typically am cutting soft and hardwood plywood designs which have several slip-fit loop and peg joints.

Without a way to stiffen my machine easily (it has the stiffener upgrades that they offer with the kit installed), my thoughts are modifications in the cut paths I use to make the pockets (a 2D adaptive followed by a 2D contour with finishing passes).

Can I add a tool adjustment that will only affect these 2x toolpaths and not the others?

Can "Spring compensation" be estimated with a negative tool wear setting? (apologies for not being very familiar with these settings).

Thanks in advance.

[jasshrie]

Ok, I've watch a few tutorials on G40, G41, G42, G43, G44 (Autodesk YouTube channel) and saw how these could be used to compensate only to learn that my machine doesn't support G40 codes.

I'm guessing that I may work around that by creating a new tool (based of the other tool I frequently use) with a slightly different diameter so as to simulate a tool wear offset, and using that for these final inside pocket contours.

Am I missing an easier way to do this?

Thanks again-