CamBam 3D problem still bothering!

[kievari]

Hi,
Still strugling by a problem with g-code generation from Inventor created STL file, in CamBam.

My files are in the attachment.

I have wood with thinckness 6mm, I designed a tablet with fillet on upper side (as a sample object) in Inventor and exported the STL file, to hopefullY generate g-code of it, in CamBam.

After importing, I used the tutorial on youtube:

‪Cambam 3Dprofile‬‏ - YouTube

‪Cambam 3Dprofile‬‏ - YouTube

The thing is that, the object in the yotuube video, after setting parameters of 3D profile, is surronded by toolpath that is matching the object boundary, but my object receives toolpath as if going far from the object boundary.

I still did not get the g-code to send to cnc machine, I fear that it will cut yet lower the depth of my wood. I set the depthIncrement on 3mm, and the targetdepth = -6mm as my real wood is.

Could anybody please help so I get out of this problem?

[Starleper1]

Okay, a couple things. I'm not sure why you have the StockSurface set at 8mm but it should be zero. Your part is already positioned so that the top of the part is at Z0 so your good there. This is the normal practice. Setting this value to anything more than zero will result in a lot of air cutting.

The next thing you need to do is re-size the part. If your click on the model from your file and then click Tools:Get Object Extremas, you will see that your model is much smaller then when you designed it. From your post, you said your part is 6MM thick.

Click the model then right click, Transform:Resize. The resize dialog box will pop up. Make sure the 'Preserve aspect ratio' is checked to keep everything proportional. Simply type 6 in the Z then apply and everything else will automatically update. So if I assumed correctly your part should measure 20x20x6.

The last thing to do is to define your stock. This is pretty straight forward and needs little explanation. If your unsure about how, I can go into detail for you.

Now just setup a 3D MOP as normal and everything should work out.

The main issue was that the part was so small that it made the tool path look huge and out of place. Now I'm not sure what size cutter you had in the MOP but I attached an example with a 3mm end mill 50% step over.

If there's anything else I can do let me know.

[kievari]

Thank you very much Starleper1! I now got clear why that happened. I would like to ask some questions please:

>I'm not sure why you have the StockSurface set at 8mm but it should be zero.
Just based on the video tutorial you see on my post. Unfortunately, I failed to find a short book/tutorial on CNC concept/terminology. I greatly appreciate if you point me to some terminology tutorials please?

>The next thing you need to do is re-size the part.
So that means that when exporting from Inventor, the STL file didn't contain the right sizes which I set in Inventor environment? As I had the right constants already set in Inventor 3D model!

>The last thing to do is to define your stock. This is pretty straight forward and needs little explanation. If your unsure about how, I can go into detail for you.
Yes please! If possible, please explain the "stock".

>Now I'm not sure what size cutter you had in the MOP but I attached an example with a 3mm end mill 50% step over.
I am using a simple drill bit of 3mm. If possible, please let me know of "step over" too.

I'm really thankful for your help and this modified attachment you sent!

Edit:
I just generated toolpath from the file you kindly attached, and got the blue lines as I expected, but the red lines are high off the object surface. How this could be explained? I attach a quick image.

[tracyranson]

Originally Posted by kievari Hi, Still strugling by a problem with g-code generation from Inventor created STL file, in CamBam. My files are in the attachment. I have wood with thinckness 6mm, I designed a tablet with fillet on upper side (as a sample object) in Inventor and exported the STL file, to hopefullY generate g-code of it, in CamBam. After importing, I used the tutorial on youtube: ‪Cambam 3Dprofile‬‏ - YouTube The thing is that, the object in the yotuube video, after setting parameters of 3D profile, is surronded by toolpath that is matching the object boundary, but my object receives toolpath as if going far from the object boundary. I still did not get the g-code to send to cnc machine, I fear that it will cut yet lower the depth of my wood. I set the depthIncrement on 3mm, and the targetdepth = -6mm as my real wood is. Could anybody please help so I get out of this problem?

If you email me your file and tell me what you are trying to accomplish I can try to help you out and email the fixed file with instructions. Email file to knottywoodcrafts@live.com

[kievari]

Originally Posted by tracyranson If you email me your file and tell me what you are trying to accomplish I can try to help you out and email the fixed file with instructions. Email file to knottywoodcrafts@live.com

Hi,
Thank you! I just emailed the file and same thing I explained here to the give address.

[Starleper1]

Just based on the video tutorial you see on my post. Unfortunately, I failed to find a short book/tutorial on CNC concept/terminology. I greatly appreciate if you point me to some terminology tutorials please?

I didn't watch the video but using anything other then zero just doesn't make sense. What this does is tells CamBam that you have stock you want to remove above the Z0 plane. When you touch the tool off the top of the stock to be machined and set Z0, this is where you want to start cutting. All your cuts will be in the negative direction. With having the StockSurface set to 8mm, it will start cutting at +8mm all the way to -6mm. But from +8 to 0 there is no material to be cut, and it will just cut air.

Unfortunately, there's no short of CNC. It's not something you will pick up over night. It takes a lot of years of experience to become a good programmer/machinist.

So that means that when exporting from Inventor, the STL file didn't contain the right sizes which I set in Inventor environment? As I had the right constants already set in Inventor 3D model!

Usually when you export STL files and import to other software such as CamBam the sizes will change. It's no big deal, you just need to re-size the model.

Yes please! If possible, please explain the "stock".

Okay, stock refers to the shape of the material before you make any cuts. CamBam only shows rectangle or square stock. It's good practice to show the stock so you can better see what will happen when you machine the part.

When you create a MOP of any kind CamBam automatically creates this MOP under a "Part" in the design tree. By default it's named Part1. If you click on Part1 you will see under the 'General' category there is 'Stock' with a little + next to. Use the + to expand the sub category. Under this sub you will see more options. Material/Stock Offset/Stock Surface/Stock Size/Color

Material- I just use this for reference, it can be used with styles but it's not necessary to set this. You can just leave it blank.

Stock Surface- This is the same as we discussed before. It's where you want the top of the stock to be. Generally 0

Stock Offset- This is used to position the stock on the screen. You can expand it and type in the values for X and Y, or just type them in as (X,Y)

Stock Size- Simply put, it's the size of the stock you have. For instance if you had 20mmx20mmx10mm stock, you would type in 20 for X and Y and 10 for Z. As you put your sizes in your will see it update on the screen.

Color- This is just to change the color of your wire frame stock.

Take a look at the stock properties in the file I attached before. Change them around and see how it effects the stock. It's pretty simple really.

I am using a simple drill bit of 3mm. If possible, please let me know of "step over" too.

A drill is not going to work for milling. You need to use an end mill. Usually a ball mill for 3D work like this.

Step over is set at the bottom of the MOP properties as a % of the cutter diameter. 0-1 or 0 to 100%. For instance if your using a 3mm cutter with a 1 (%100) step over, every time it makes a pass and steps over to make the next it will move 3mm. If you use 0.5 (50%) it will step over 1.5mm, and so on.

For roughing it's good to take larger step overs. When you go to do the finish pass you will need to use a small step over to achieve a nice finish.

Edit: I just generated toolpath from the file you kindly attached, and got the blue lines as I expected, but the red lines are high off the object surface. How this could be explained? I attach a quick image.

The red lines are your rapid moves to the clearance plane. Which in the file is set to 10mm. You can leave it set at 10mm and set your FastPlungeHeight to something like .10

Hope this helps.

[kievari]

Thank you very much, lot of things now clear to me...

By "short on CNC" I meant a book someone wrote with deffinitions like yours:
>...stock refers to the shape of the material before you make any cuts.
I'm clear forever on what stock is!
I mean a book of such deffinitions, not tutorial/how-to, just to exactly know what is what.
My use cases on CNC machining are pretty trivial: currently trying to create wooden constructions for hobby robots around second hand printer motors! I hope that in 1 year to learn to do them good.


>...A drill is not going to work for milling. You need to use an end mill. Usually a ball mill for 3D work like this.
Seems I'm missing something here, could you please check if I'm understanding you well here please? I found these on ebay:
End Mill
Ball End Mill

>...The red lines are your rapid moves to the clearance plane. Which in the file is set to 10mm.
Where I can see that in file please? How can I change it to 0 as like by default please?

>Hope this helps.
More than just help, your text teaches excellent

[Starleper1]

I mean a book of such deffinitions, not tutorial/how-to, just to exactly know what is what. My use cases on CNC machining are pretty trivial: currently trying to create wooden constructions for hobby robots around second hand printer motors! I hope that in 1 year to learn to do them good.

Check this link out. It should give you more than enough information.

CNC Programming Handbook

Seems I'm missing something here, could you please check if I'm understanding you well here please? I found these on ebay: End Mill Ball End Mill

Yes those are correct. Standard twist drills are only used to make holes. Nothing else.

Glacern has a great crash course in milling for beginners. Check it out.

Where I can see that in file please? How can I change it to 0 as like by default please?

You don't want to change it to 0. This is the clearance plane. What this does is tells CamBam where to go after a MOP is finished or in between levels of a pocket etc...

For instance say you have a series of holes to drill. When you hit cycle start the machine will rapid to the clearance plane first, and then move X&Y to the position of the first hole and begin drilling. After the first hole is drilled it will rapid up to your clearance plane and then move X&Y to the next hole position. And so on. If you were to set it to 0 then there would be no clearance between the tip of your drill and the top of your part.

Have a nice day.

[kievari]

Hi,
Thank you very much for detail responses, support and accurate information and resources, my question is fully answered. Thank you again

[Starleper1]

Not a problem. I'll help support CamBam any day.

Glad I could help.

[tracyranson]

Originally Posted by tracyranson If you email me your file and tell me what you are trying to accomplish I can try to help you out and email the fixed file with instructions. Email file to knottywoodcrafts@live.com

The red lines that you are refering to are created when you input your clearance plane data. The higher the number the taller the your clearance plane will be. The clearance plane could also be refered to as the z-safe zone that the Z axis will retract to. Your clearance was set to 10 if you set it to .50 you will notice that the red lines will shrink down to .5" above the zero or top of the work piece. I hope this helps.

[kievari]

Originally Posted by tracyranson I hope this helps.

Sure helped thank you! I learned this term: " z-safe zone"

I now imagine it better: the cutter after a MOP moves up to the "z-safe plane" and on that "plane" moves to the next MOP position, then again down to do the stock to do next job.

I'm feeling a happy newbie now