milling problem

[chip1964]

Hey everyone!

I hope i am doing this right? I have a 3d model that i imported from soliworks and programmed it using featurecam. When i view the program in 3d mode with show gouge settings on there is no problems. But when i run it in my fadal 15xt it puts marks in the part. The part has some 3d faces to it and they come out fine it is the 2d milling that is the problem. picture an angel wing i am milling a pocket .125 deep thats okay the outside of the wing is a side milling operation .019 deep. when it does the side mill it puts a mark in the part. there are 8 different sizes and i have programmed them the same 4 are okay 4 are not. Featurecam tells me the post is good and the backploted it and said there is no problem. fadal replaced 2 resolvers and i still have the problem. They tell me becouse it is dc drives it is not reading the post fast enough. they told me to take out all the arcs and put lines which made the program 2.5mb and three times longer. Then they tell me that they have seen this random problem in the machines before and tell me that i need to upgrade to a fanuc controller. i have been using the software since 1997 and have never seen this problem does anyone have any suggestions.

[Paul_S]

Have you tried slowing down the feed for insided arcs? The simple method: inside arc feed = linear feed x (inside arc radius - tool radius) / inside arc radius. Then return to linear feed coming out of the arc. For finishing the equation becomes: inside arc feed = linear feed x square root ((inside arc radius - tool radius) / inside arc radius).

If you uses linear moves to simulate arcs make sure G8 is turned on and that G9 is returned for your positioning moves.

Finishing moves, may need two finish passes do to materal and tool deflections.

It all depends what is the cause and reason for the gouging.

[fpworks]

How is the feature created in Solidworks? Are all the arcs tangent to one another? Are you using splines or data points to create the pocket geometry?

I had a similar experience using a complex curved 2D part created with Pro/E and programmed with OneCNC. The part geometry was 2D, defined by a splined curve through a series of points. The model looked perfect, I had absolutely no problems programming it, but the machine left a tool mark when it was machined. Later I discovered that this tool mark occurred at the point of spline intersections. (BTW, the spline intersections were trimmed and tangent)

The only way to remove the tool marks was to replace the spline with a defined arc that approximated the the splined curve.

You may want to see if your tool marks have any correlation to how your model was constructed/defined.

When the machine was running this part, I noticed a very brief slow down in feed rate as it passed these points...that is when I started investigating the model.

Hopefully my experience will help.

Justin

[chip1964]

I want to thank those who replied. We have chosen an alternate route. We purchased a new supermax 1020a with a fanuc 21i-mb cntroller. We asked a few other professionals and they suggested this company. I asked fadal to cut a part on one of there machines with my software and they told me that they did not want to do it with there controler. They said that it would not be a fair test becouse it may cut right the first time but not cut right the next. They wanted me to cut it in a 4020 with a fanuc 18i controller. I like the fadal machine format 2 is a breeze But my customers come first. We are keeping th 15xt for light duty 2d work since it is paid for and does not call in sick or complain. The cam software i use has been very productive for me. I agree with them when they say how can you be a major player in the market if you cant cut circular interpolation. Telling me to take out all of the arcs and rplace them with lines costs me money.

This is my opinion

Again thank you!