Featurecam 2019 problem with stock with irregular shape

Hello, fellow machinists. We make some plates out of 10mm aluminum with a lot of holes and taps in them with +/- 0.1mm position tolerance. Since we use the "fast" cut technology table on our fiber laser sometimes their dimensions are out of tolerance and I decided to cut them 2mm bigger in every dimension on the laser and after that cut them to dimension, drill and tap them on one of our VMCs. Our programmer is on a long leave and I can't seem to figure out a way to make FeatureCAM understand that I don't want to cut it from a block of aluminum but rather a bigger version of the part itself. Does anyone have an idea how to do it easy or should I have someone make a solid model just for the stock? Thanks in advance for the replies.

Best regards

If I understand correctly your stock is 2mm o/s , you can set your stock that size and machine your profile around the part and your profile will cut to size. Featurecam recognizes your stock size and cuts accordingly. If you draw your part out you will need to add your stock size per one side(1mm in your case) to draw your hole location. Hope this helps.

This is exactly what I want to do but Featurecam only gives me the options to pick between a rectangular or round stock, not something with complicated contours.

anht said:

This is exactly what I want to do but Featurecam only gives me the options to pick between a rectangular or round stock, not something with complicated contours.

Click to expand...

Keep going......after you choose rectangle stock it will allow you to define the stocks shape/size.
Double click right on the stock and the window will open.

If you just want a finishing pass, look in the last tab where you set parameters like number of finish passes. There should be a *stock allowance parameter. If you set it to .030 featurecam will ignore the actual stock and assume that there is only .030 on the profile you selected and it will cut accordingly.

Its quick and dirty but works well especially for simple stuff.

*Sorry I'm not in front of the computer and don't remember the actual name of the parameter.

Edster said:

If you just want a finishing pass, look in the last tab where you set parameters like number of finish passes. There should be a *stock allowance parameter. If you set it to .030 featurecam will ignore the actual stock and assume that there is only .030 on the profile you selected and it will cut accordingly.

Its quick and dirty but works well especially for simple stuff.

*Sorry I'm not in front of the computer and don't remember the actual name of the parameter.

Click to expand...

I think you are referring to the 'Total Stock' parameter.

Fred

Yupp, do as Wheelie and Edster suggested.

First, just go through the normal procedure of defining your stock and the part within it.
Then, create a curve from the outline of your finished part.
Then offset this curve by say 2mm to the outside, which will leave you with another, separate curve.
Then go back into the STOCK properties dialog, click on Stock Curve and select the newly created, offsetted curve as the stock.
Done.

Now, when you go to actually machine the contour, for the Rough or Finish operations under the Milling tab you will find a parameter "Total Stock", enter something relatively small enough
(the 2mm would be sufficient ) so your will get only one pass on the contour and not remove anything else on the outside.


Sometimes you gotta love FC.
Someothertimes .... not so much.

Yup, total stock. I couldn't remember off hand what it was called.

I don't think you have to use a stock curve if your using total stock though. Just draw the profile you want to cut and enter the total stock value.

Edster said:

I don't think you have to use a stock curve if your using total stock though. Just draw the profile you want to cut and enter the total stock value.

Click to expand...

Edster

You're correct of course, you do not need to modify your stock, the Total Stock setting is all you need.
Except, the older I get the more I forget.
I keep spending more and more time remembering how did I do this just a few weeks ago? Why did I do that? Who did it? What?

So, as part of my documentation I started spending some time creating exact setup sheets not only on paper, but in CAM as well.
It was OK when it was just me setting stuff up, but since now there are more of us, I'd rather just have them look at the screen and leave me alone not having to explain things.

In case of the OP's issue, he sometimes have a solid block to cut from, sometimes a finished contour, and now he's got a near-net shape.
In this situation I just duplicate the CAM file, make the changes to the stock ( or whatever else ), document it so the Dumbass ( me) will not loose any hair the next time around.

SeymourDumore said:

Sometimes you gotta love FC.
Someothertimes .... not so much.

Click to expand...

There are only two times I hate FeatureCAM.
Anytime you have to include autodesk (like a freakin' sucker I paid my maintenance yesterday )
Trying to manipulate 3-D tool-path. Sometimes I struggle greatly working in 3-D.
Any other time? FeatureCAM rules!

SeymourDumore said:

Yupp, do as Wheelie and Edster suggested.

First, just go through the normal procedure of defining your stock and the part within it.
Then, create a curve from the outline of your finished part.
Then offset this curve by say 2mm to the outside, which will leave you with another, separate curve.
Then go back into the STOCK properties dialog, click on Stock Curve and select the newly created, offsetted curve as the stock.
Done.

Now, when you go to actually machine the contour, for the Rough or Finish operations under the Milling tab you will find a parameter "Total Stock", enter something relatively small enough
(the 2mm would be sufficient ) so your will get only one pass on the contour and not remove anything else on the outside.


Sometimes you gotta love FC.
Someothertimes .... not so much.

Click to expand...

yup.. that's the way I'd do it. was going to explain it the same way as Saymourdumore until I saw his post... so "what he said"