Is there a hard and fast rule as to when to use either option when setting up toolpath settings? I have version 20.7 and have been through the videos that came with the software but I dont recall any instruction on this. i have had this software for about a year and a half, have done a ton of work with it but I am just starting to play with the 3-d stuff.
Also, do these options come into play when using a bullnose cutter?

These options are only used when you have a boundary around your part.

There is a differene in the Toolpath that is generated.

When you use the Tool Edge (Outside of Tool), the toolpath that is generated is compensated to the inside of the boundary for half the cutter diameter. That means that the Outside Edge of the Tool will come in contact with the boundary and that is all.

When you use the Tool Center option, the toolpath will not be compensated for the cutter diameter. This means that the center of the tool will come in contact with your defined boundary.

Regards

Thank you for the response, but I used the wrong terminology in my question.

What I meant to ask was about the "toolpath repersent" options in the solid toolpath dailoge box. What are any rules used to govern "tool center" or "tool tip" and does using a bullnose cutter have any certain rules when deciding which to use?

These options will not influence the toolpath when using a Bullnose or Flat end mill. These options only apply to the Ball End mill option. When Tool Tip is selected the resulting toolpath will be based off of the tip of the Ball. When Tool Center is selected the resulting path will be offset in Z for half of the cutter diamter.

Regards

That explains a lot, like why my toolpaths havent been going all the way to the bottom when using the "incorrect" option and a ballnose cutter!

Gald to Help

;)

Regards

Gald to Help

;)

Regards

That's great!!!!!!!! Can you help with this one, Please?????:)

Thanks!!!!

http://www.cnczone.com/forums/showthread.php?t=31037


:rainfro: :)

That explains a lot, like why my toolpaths havent been going all the way to the bottom when using the "incorrect" option and a ballnose cutter!


When using to center option you must compensate on your machine by 1/2 the tool diameter in the Z axis. Your ball wndmill will then go all the way to the bottom of the part. Be warned though, the Z position in the post for the part top should be an addition of half the tool as well.

I don't have any idea if I can explain this well or not but the tip or center option does about a million more things than I've heard mentioned, I own a company that builds exotic wheels. I don't have expensive software for a reason and one of those reasons is Bob cad is kind of a 'dumb' program if you will. (You can lie to it A LOT to get the desired result if you know how too. Let me explain...)

An easy one to start with (without lying to it) is thinking about cutting with the center, (math geeks forgive my terminology!) If you have the latest version of Bob cad, you have an option called "project curves on surface". Let's take an imaginary contoured form with irregular smooth surfaces. Now above it take a 2D image (lettering for instance) you'd like to engrave and place it above your part in Z. Now click the button under solids and it will imprint an image of your text on the top and bottom of your 3d surfaces. Erase the bottom ones and then select the left over top portion. Now simply have that selected and 'translate' those entities down (negative Z) the radius of your ball nose cutting tool and you're good to go. As long as you don't go over 45 degrees (I forget but that sounds about right off the top of my head, I'm tired,) slope you get the exact same depth everywhere on your engraving.

Obviously that is a very straight forward way to manually write something but when you're using the Bob cad wizards like was mentioned above there is a really cool feature you can use to make complicated shapes extremely easy.

(I'm working on a big project due in the morning so I have the radio blasting and my equipment running to stay awake, sorry about the randomness of this one guys!!)

I don't think you'll find any of this in their brochures or CD's but here goes...

Here's the secret, lie to it! For instance if you'd like to do some really cool step downs you can simply tell Bob your cutter is smaller than it truly is using the 'tool center' option and by using the border option to box in an area, you can draw path for just the step down. Then highlight it and drop it in Z the difference between your real cutter (diameter or radius I forget...) If you do that on both sides of your part as in a motorcycle wheel for instance it looks absolutely insane! (See 'talons' on the picture at the end of this post.)

If you're serious about using this option effectively, all it takes is a little experimentation but remember the two outputs are completely different. You cannot simply use 'tool tip' and then drop it the radius of your cutter to get tool center. (Seems like you could but go ahead and try it, lol, they're not my parts...) Here is a picture of some work I did tonight with just this feature...

http://www.miabc.us/news.htm

(It's a motorcycle wheel that gets brass piston rings tomorrow for a customer in Louisiana. I used the option we're discussing to VERY rapidly program the piston ring grooves to be EXACTLY .082" deep ALL the way around the pistons top, bottom and sides... It works flawless!! I'll be making the actual 2d rings later tonight along with all the inlays. There are 96 individual pieces to the front 21x2.15 and rear 18x10 wheels when completed...)

You can right click on any image to view it and then blow it up... They are 10.1 mega pixel images, lol, if you're good, you can actually dimension right off the picture... (but that's another topic for another time~)

Below is another real life example of this process in action, (it was the first wheel I ever built)...and no, I haven't found anywhere to explain in any real detail how to do it but now that you know it's possible, try to figure it out... I have about 20-30 little tricks like this I use all the time~ (Note the step downs on the 'talons'... (They are dimensionally perfect all the way around on an arc with continuously varying radii. Blended to a .020" ball point end, there was NO polish or deburring of the pointy parts before it was chromed, it came off the machine nearly perfect.) Not only that but there is 3 degrees draft on every surface of that wheel blended out into another radius at EVERY spot... (Look up threads on harmonics and 'tuning' your parts.) The piston wheels however just had to get done quick and dirty, so I polished those out by hand...takes about 7 minutes a piece...