[Megaplow]

Hey All,
Is there a feature or best practice for making little tabs to hold my parts and fall away bits? In the past I have altered my models and added tabs about .03" x .03" and made all the complex tool paths to cut around them. It seems there should be a better way.

Any advice or links on the topic would be much appreciated,
Joe

[mdlmkr]

You can put in a negative number in the Lead In Overlap setting. This setting is in the Lead In tab in the Operations Parameters window. You are only able to use this setting in contour toolpaths, so no roughing.

Hope this helped.

[my87csx481]

I am completely unfamiliar with the software (demo copy is supposedly on its way) but, I have a question related to your question: Is it possible to use models of straps/clamps and assign them as such and have a parameter to keep cutters away from such objects by a specified amount/boundary?

I've had to do quite a few parts where we move the straps mid-way through the program and finish the clamping areas when the straps are out of the way.

[Japazo]

mdlmkr,

Using the leadin/out settings works in many cases, but a failsafe is to sketch your tab and add it as an avoid area for whichever tool paths you see fit. This is more versatile as it gives you the ability to define the size, location, quantity and depth of the avoidable area without compromising the rest of the toolpath for any given operation.

my87csx481,

You can either do as I stated above for "part mode" programming, or you can insert ALL of your components into an assembly file and program in "assembly mode". Assembly mode gives you a much better way of accurately avoiding clamps and complex fixtures. I use it whenever I am cutting on my 4th axis with complex rotary fixtures in order to avoid clamps and the fixture itself. Assembly mode is a little tougher to learn and requires a few more steps, but is a life saver when dealing with complicated setups.

Hope this helps both of you!

[acannell]

mdlmkr,

Using the leadin/out settings works in many cases, but a failsafe is to sketch your tab and add it as an avoid area for whichever tool paths you see fit. This is more versatile as it gives you the ability to define the size, location, quantity and depth of the avoidable area without compromising the rest of the toolpath for any given operation.

my87csx481,

You can either do as I stated above for "part mode" programming, or you can insert ALL of your components into an assembly file and program in "assembly mode". Assembly mode gives you a much better way of accurately avoiding clamps and complex fixtures. I use it whenever I am cutting on my 4th axis with complex rotary fixtures in order to avoid clamps and the fixture itself. Assembly mode is a little tougher to learn and requires a few more steps, but is a life saver when dealing with complicated setups.

Hope this helps both of you!

i would agree with this. i have only been using camworks for a couple days and today i tried to figure out how to avoid the bolts that will be holding my stock for 2.5 axis operations. i also needed to figure out how to not exceed my mini-mills rather small working envelope of about 10" x 7".

i think ive figured both out!

i drew the bolt locations in a sketch, using circles as the size of the bolt head (biggest part). i used parametric ways of locating the bolts so that they would not interfere with the tool paths.

then, you have to make individual sketches, one for each bolt, at least in my ancient version of camworks 2001 plus.

then in the operations manager you can add them as avoid areas. right click on something.. i think its each operation (im tired). you can add an offset so the toolpath stays say.. 1/16" from the bolt heads. tada!

now if you are pushing your machines work envelope to the limit trying to make a big part(s) and coming right up to the edge of travel, just draw the machine limits as a box in a sketch, probably centered on the geometry of your part. then use it as the workpiece sketch.

some of this may or may not be the best way, but if you are a camworks noob then try it out and it might help you understand whats going on

[jame5m28]

Its pretty easy, insert an avoid area (right click on the operation, "INSERT AVOID AREA")

you can select a sketch and in the 2013+ versions of CAMWorks you can set a "height offset"

in the operation paremeters on the advanced tab you can select how you want to avoid! either around for going around a bolt, or feed over for leaving tabs....