[Ponchibego]

I'm working with a homemade router and I just got done with the fine tuning aspects (squaring, calibrating, etc). Now I'm on to doing some practice cuts on scrap wood to make sure my G-code is of quality status. Everything looks all peachy and pretty in the BobCad simulator, but when I do the real deal stuff screws up. My most recent run was supposed to perform a pocket to 1.65", but for some reason cut all the way through my stock and into my table. According to Mach it thought it was located around 1.4"", but it had really already cleared the 1.65" and was cutting additional depth. My problem is I have had this randomness of errors occurring often enough where I don't want to put my valuable mahogany on the table until I have this all sorted out. Along with any advice on this I also want to ask about two things. 1) Could using absolute distance mode over incremental be part of the issue? 2) I'm using Mach, but how do I specifically know which post processor to be using (i'm currently using Mach3-Mill-NoATC.MillPst)?

Thanks in advance

[The Engine Guy]

I'm working with a homemade router and I just got done with the fine tuning aspects (squaring, calibrating, etc). Now I'm on to doing some practice cuts on scrap wood to make sure my G-code is of quality status. Everything looks all peachy and pretty in the BobCad simulator, but when I do the real deal stuff screws up. My most recent run was supposed to perform a pocket to 1.65", but for some reason cut all the way through my stock and into my table. According to Mach it thought it was located around 1.4"", but it had really already cleared the 1.65" and was cutting additional depth. My problem is I have had this randomness of errors occurring often enough where I don't want to put my valuable mahogany on the table until I have this all sorted out. Along with any advice on this I also want to ask about two things. 1) Could using absolute distance mode over incremental be part of the issue? 2) I'm using Mach, but how do I specifically know which post processor to be using (i'm currently using Mach3-Mill-NoATC.MillPst)?

Thanks in advance

First of all which version of BobCAD are you using V23/V24/V25 ? ?


None of the Post Processors work 100% out the box, they all need a little "tweaking" and the Mach3 posts do need quite a bit doing. I have attached a Post Processor that is known to work

Nothing wrong with working in absolute mode (G90) as long as you have setup your Mach3 correctly and most importantly have you set your tool and top of stock correctly in Mach3 ?

Can you post here one of your BobCAD test programs, just Zip it up and use the "Manage Attachments" facility to upload, that way it will be easier for someone to see if there is a problem with your program

Regards
Rob
:rainfro: :rainfro: :rainfro:

[ger21]

According to Mach it thought it was located around 1.4"", but it had really already cleared the 1.65" and was cutting additional depth.

If the actual position does not match the position on the DRO, then the machine is losing or gaining steps. This is usually caused be trying to move faster than the motors are capable of.
Try reducing the acceleration by 50%. You may also need to reduce the velocity.

[Ponchibego]

The Engine Guy: I'm using V24 and below I attached the exact file I was working with.
Ger21: I don't know what the standard for acceleration is but I have it already set at 1 which seems low to me and my velocity is at 70 IPM. I'm certainly newbish to this still, but both those numbers to me sound reasonable especially since I can get my router to travel at 200 IPM before "stalling" occurs. I hope the word stalling makes sense since there's no other real way I can think of describing it.

[The Engine Guy]

The Engine Guy: I'm using V24 and below I attached the exact file I was working with.
Ger21: I don't know what the standard for acceleration is but I have it already set at 1 which seems low to me and my velocity is at 70 IPM. I'm certainly newbish to this still, but both those numbers to me sound reasonable especially since I can get my router to travel at 200 IPM before "stalling" occurs. I hope the word stalling makes sense since there's no other real way I can think of describing it.

OK, I think I have it, your stock is 1.5500" thick and you had pocket 2 (The small round one I think) set to a depth of 1.625", that will certainly go right through your stock

You had also selected geometry for both pockets for both "Feature Pockets" so although you had pocket 1 set to 0.1500" because it was also selected for pocket 2 that would also be cut right through

I have modified the program to what I think you wanted but if it`s not right then I can easily alter it for you. Take a look at the attached file and try using the attached Post processor in the other Zip file, I think it will be closer to what you need than the one you are using. I have generated the code from that Post and run it through my Predator backplot and it runs true. As you were using the same size tool for both roughing and finishing I have altered the program to take account of using the same tool

Regards
Rob
:rainfro: :rainfro: :rainfro:

[Ponchibego]

We're good to go! I tried both my old code and your new code along with the adjusted acceleration. Both codes worked just fine and I think my primary issue was that I was gaining steps. Thanks again for the help.

[jrmach]

Stock of 1.5500 with a cut 1.625 in depth,is going to be a problem each and every time,as Rob pointed out.

[Ponchibego]

The BobCad stock depth is a little misleading because the actual board I was cutting is 2" thick. I will update my stock depth just so that it matches the stock depth in reality.

[mmoe]

If you have Mill Pro, you can pretty easily do this in 3d with the benefit being that you machine off of the surfaces. Mill Pro give you the Flatlands feature, which Mill Standard doesn't have and makes pocketing routines easy in 3d. When machining off of the 3d parts, you don't really have to set the depth of cut, since that is dictated by the model of the part itself. This makes for a bit less opportunity for error when it comes to pocketing depth. If you have Mill Standard, it can be done in 3d as well, but not quite as easily.

Generating a 3d model from your 2d part only takes a couple minutes (literally) in ViaCAD 2d/3d V8, which you can get for $35 on Amazon. I've been wanting to try making a video using AutoScreenRecorder to see how it works, so this seemed like a good time to try it. Here is your part rendered as a 3d model (in metric though, as that's what I'm used to working in). I just made some arbitrary thicknesses of 40mm, 36mm and 8mm to create pockets that are 4mm and 32mm deep from the top of stock. I edited out the tool path generation in the video to shorten it, but if I hadn't the entire process of creating a 3d model from the 2d drawing, and then generating the needed toolpaths was only a total of 6 minutes. So I wouldn't say it's a whole lot more work or time invested than using the 2d methods, but with the benefits a 3d model offers.

3d Pocketing in Bobcad V24 Mill Pro - YouTube

[RAF.]

Your video sure looks good from here what version of AutoScreenRecorder is that.

[mmoe]

Thanks! It's release number 3.1.375

It gave me trouble if I tried to record at anything more than 12 or 15 FPS though, so as long as you keep it slow it works pretty well. There were a couple of times when it felt like it made the software stutter a bit compared to normal use, so any stuttering in the video is a result of the capture, not ViaCAD or Bobcad. The slower you run it, the less of that you get but then you get gittery mouse motion. That's the first time I've tried a screen capture video, so it was fun to play with.


I forgot to mention earlier that if you don't have Mill Pro, it still is useful to do the 3d model. If your tool path is incorrect, you'll see that because it doesn't match up with the model. If you ran a 2d pocketing feature and it was set too deep, it would show the tool path coming out the bottom of the model and you'd know it was wrong right away. Once you get used to pulling the edges off of the 3d part, it's very easy to work with a 3d model using 2d techniques as well as the 3d techniques. I think that if I had Mill Standard, I'd use the 3d roughing feature first, then run two 2d pocketing features for the two different levels of pockets. For the pocketing features, you wouldn't need to step the pocket in since the roughing already removed that material. There would be some cutting in air for the upper pockets (unless you drew or offset more geometry from the inner profile) which isn't there if you have Mill Pro and use the Flatlands feature. Regardless, I've come to believe that having the parts modeled in 3d is very useful for verifying that you're getting the tool paths you want.

Edit: Here's another video of the same 3d model with both the 3d roughing feature and two 2d pocketing features for those that might be working in Mill Standard. I ended up offsetting the upper pocket profile towards the middle so as to create a boundary of sorts for the upper pocket and reduce how much air is cut. The step over of the pocketing is set at 75% since the roughing feature left only 1mm to cut. I also set the pockets to do only a single pass, again due to the roughing feature having removed most of the material already.

For what it's worth, it took a total of 6 minutes to generate the model and the toolpaths in full 3d using Roughing and Flatlands features, but it took nearly 6 minutes just to create and generate tool paths using the same model, but with 3d Roughing and 2d Pocketing features (not including the 2d to 3d modelling in ViaCAD). Even though it takes longer for the tooppaths to generate in 3d (once you have created the feature), the time saved by Flatlands vs. Pocketing more than makes up for the additional time it takes to generate because Flatlands will do all of the same processes in one feature as multiple Pocketing features would otherwise be necessary to achieve. Watching the progress bar while Flatlands is processing makes it seem like Pocketing would have been faster (since it is nearly instant), but the saved time in creating one feature instead of multiple features more than makes up for it. Either way, I think this also illustrates that a 3d model can be just as easy to program off of as the 2d drawing, but give you that extra bit of visual verification.

https://www.youtube.com/watch?v=C-XsbAkMMjs

[Ponchibego]

So the code we worked on before is working good, however I've moved onto the next code for the guitar and I'm having some issues as shown in the attached pictures. It appears that it's cutting nice straight lines, however when the finishing job comes around it leaves these weird divets in the cut.

[jrmach]

Can you share a file ?

[mmoe]

How deep is the cut and what is the tool cutting length? Did the smaller pockets within the larger pocket get cut first? If that is the case, it looks a little like the finish pass was too tall for the cutter and it deflected the bit away from the pocket. The corners would show the cut because the bit plunged there, but as soon as it starts going in a direction, the bit essentially traced the pocket instead of cutting new material. The top bit of the material also looks a little like it got scorched from friction, but it's difficult to tell in photos.

[Ponchibego]

Yeah I was worrying that perhaps it was due to deflection plus my gantry has a little flex to it. I don't see how I could fix the flex in my gantry with the design of my frame and will just have to accept that. My finishing pass is set at 0.05", do you think it would work better if I set that to something larger like 0.1" or 0.125" so that it has a little more surface to contact to reduce deflection? Note I'm working with a 0.25" diameter bit.

[RAF.]

I know you don't probably want to hear this, but what about slowing the feed rates down , might be worth a try.

[Ponchibego]

I can try that... I have enough scrap wood to do about 10 tests. I currently do rough passing at 70 IPM and finishing at 30 IPM, but I can certainly drop that down to say 15 IPM.

[jrmach]

Sooooopoo,the file you just posted is not the file you are using?????
Cause what RAF just pointed out is the first thing that jumped out at me.Something like 175 ipm,,
See if slow things down a bit if that helps.Other than that,the problem is going to lie outside the program.Let us know.

[jrmach]

I am thinking you would benifit with posting here DIY CNC Router Table Machines

You said you just got it up and running,,my gut feeling is you have some work still to do on machine.