Why my model doesn't work properly in practice?

[firanman]

Hello everybody,

I've designed a flat-dog-bone-shaped specimen in Fusion 360 to generate a G-code for the CNC mill. when I run the simulation both on Fusion360 and on my CNC machine everything looks fine but when I run the real simulation it gives me the following specimen:

what I designed is as follows:

So as you see, 2 of 4 edges have not been milled properly. I was wondering to ask if anyone can help me solve this problem. I guess there is a tool compensation parameter that I missed and I don't know how to account for that. I have attached my .f3d file as well. I'd really appreciate your advice.

[HughesTooling]

Is this the correct file? It looks like the one I helped you with the correct way to select the whole profile. Also working from a mesh is not really a good idea and will not create a nice toolpath of simple arcs and lines.

[firanman]

yes, it is the same model. I don't know why it doesn't save the correct toolpath. I need to select the closed one every time (that issue was solved with your help and I'd appreciate that). Could you please help me to remove the mesh? I don't know how can I delete mesh. I saved it in a new f3d file. Could it be a tool compensation issue? because the gauge width is larger than the real one as well.

[HughesTooling]

Working form mesh files is not a good idea as you end up with G code that's made up from short lines and arcs so avoid STL files.

You need to figure out how to draw this in Fusion, have you done any of the tutorials?

Start with these.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-962B7698-D862-4D7D-AB33-EEE39542DD2F

Then try drawing up your dog bone and if you get stuck come back to this thread and post your model for advice.

[HughesTooling]

---

@firanman wrote:

I don't know how can I delete mesh. I saved it in a new f3d file. Could it be a tool compensation issue? because the gauge width is larger than the real one as well.

---

You have the op set to In Computer so the path is offset so no compensation needed in the control. You did use the same size cutter on the machine as you set in Fusion?

This should have worked but what control does your CNC have? Because you worked from a mesh the G Code will have lots of short moves, some arc some lines. Some controls can have problems if there are lots of arc moves like this. Best if you can redraw in Fusion as a proper solid model then try again.

Mark

[HughesTooling]

I didn't really want to draw this for you but there are some bad habits you might get even following the tutorials.

When sketching keep the sketch as simple as possible and avoid filleting in the sketch. This part also has symmetry in two direction so you only need to draw a quarter then mirror. I've attached the file and updated the CAM. You can edit the features in the timeline to get an idea of how it's built. If you edit the sketch you can double click the dimensions you can change the sizes. I'd still recommend you go through the tutorials.

[HughesTooling]

@firanman  It dawned on my the part might have moved when it cut through. I see you'd enabled tabs but the distance was too big so you didn't have any!

I've edited the operation and set to At Points and select the midpoint at each end. I've also set the lead to ramp so it's not plunging in. What material thickness are you cutting the part from, you've set the stock to 4mm in the setup. This will need to be correct for the tabs to work. See attached file.

[firanman]

Thanks @HughesTooling for providing this. I ran it using my CNC machine as well and I ended up the following:

However, with this last one, I think I used a cutter with one size bigger than what I assigned in the software.

[firanman]

Hello,

I've created a new model with some changes but I don't know why it cannot cut all the way through this. Although my stock height is larger than my sample height I want it to cut all the way down.

[HughesTooling]

---

@firanman wrote:

Thanks @HughesTooling for providing this. I ran it using my CNC machine as well and I ended up the following:

However, with this last one, I think I used a cutter with one size bigger than what I assigned in the software.

---

It looks like the part has moved because the stock thickness was probably wrong so it cut through the tabs.

I've made a screencast fixing your second model and set the bottom depth to Stock Bottom -1mm, make sure this matches your stock thickness.

Your sketch is not done well, you've drawn it at a random place rather than fixed to the origin also you should not draw fillets in the sketch as it's easer to constrain and dimension with sharp corners. Design's attached.

Mark

[firanman]

Hello @HughesTooling , Thank you so much for providing this for me. You mentioned a very good point about the stock thickness which may be the source of error. Just, I don't understand why should I fix my model to the origin? Also I didn't understand why shouldn't I draw fillets in the sketch?

[HughesTooling]

---

@firanman wrote:

Hello @HughesTooling ,

You mentioned a very good point about the stock thickness which may be the source of error. Just, I don't understand why should I fix my model to the origin? 

---

You should always anchor one point of your sketch to a fixed point. As this is the first sketch in your design your only option is the origin. Fusion's sketches are parametric, if you want to be able to edit sizes and get a predictable outcome you should fix one point then fully dimension all the curves.

---

Also I didn't understand why shouldn't I draw fillets in the sketch?

---

To fully constrain a sketch with fillets is a lot more work. If you can design the sketch with sharp corners then add the fillet to the body it's a lot easier to manage.

Here's an example of why you should fix a point to the origin, keep the sketch simple and fully constrained.

I changed the width in your sketch from 11 to 12mm and this happens!

If you do the same with my simple sketch everything resizes predictably. Also note the red padlock on the sketch that indicates the sketch is fully constrained.

Mark

[firanman]

Thank you so much @HughesTooling . That makes sense.

regards,

Faezeh

[firanman]

Hello @HughesTooling . I have a question. Why did you choose the following tabs?

[HughesTooling]

---

@firanman wrote:

Hello @HughesTooling . I have a question. Why did you choose the following tabs?

---

Are you asking about shape or position? Shape I chose because the angled sides mean the cutter with ramp down rather than plunge straight down. The angled ramp will cut easier. As for position, just thought the 2 ends were the best place, you might find you need 2 more on the narrow section if it still moves.

Mark

[firanman]

I asked about the existence of the tab (I mean why you chose to have tabs) but based on your explanation what I understand is that you chose to use ramp cutting. But when we have tabs, there is some remaining material that is not removed and I need to do another cutting to remove these parts.

[HughesTooling]

The reason for the tabs is you need to hold the part in place when the cutter takes the last cut around the part. I'm pretty sure the problems you had with missing corners on the finished part was because it moved.

How are you holding the stock down?

Mark

[firanman]

Hello Mark,

Actually, I use two grips to hold the stock but in the last round, as you said, the sample moves. But this problem with corners starts from the first round before that sample starts moving. 

regards,

Faezeh

[HughesTooling · Accepted solution]

What machine and control are you using and have you got the correct postprocessor? Even if you used the wrong cutter it should still be consistent, all corners should be the same. A wrong sized cutter would only make the part the wrong size. 

Different CNC controls can specify circles and arcs differently so you need to make sure your postprocessor and control are set the same.

Try the attached file. I've modified it so there are no arcs on the part or in the toolpath.

Mark

[firanman]

Hello Mark,

I am using the Sherline CNC mill (https://www.sherline.com/cnc-for-sherline-machines/). The post-processor is LinuxCNC (I checked it with the company), but I don't know about the control. I was thinking the same and thank you for the file that you kindly provided for me. I will try that the next week and let you know if that worked. Thanks for your assistance in advance. 

Faezeh