FeatureCAM code problems

GisMo · Feb 25, 2005

The toolpaths look good on the computer, then i take the code to the control and run the code again. 85% of the time the code is good, the rest, it will randomly throw in some circles in the tool paths that just seem to ruin everything. It's a pita on longer programs to run through and delete the lines that are bad..But last night I ran in to some new problems..I caught the circles and just deleted them, ran the program and on some of the finish pass, it seemed to have ran a secant line instead of finishing around the arc..those errors aren't like the circles where I can delete it out..these just baffle me..I dont know how to fix the secants other than messing with featurecam and changing the program and regenerating the code, in hope that they are gone.

Any ideas? any software that will run the code on the computer?not cam, just software that will show me the code for ease, besides running it on the controller.

Thanks in advace... I will post pics of the reuined part later today.

harrytm · Feb 25, 2005

It sounds like there are lines in your geometry that are shorter in length than the offset you are introducing in your CAM. I would suggest that you try running .0000 offset and see if that takes care of the troublesome circles. If it does, then tahat's your problem. You would either have to go back and change your geometry. Some cam programs will allow you to "blend" entities and basically change the toolpath so you won't get your circles.
Another option is to offset your program the amount of your offset so you can run a zero offset at the machine.

GisMo · Feb 25, 2005

Which offsets? Somewhere in featureCAM? As for a stock offset, part origin is the center of the stock. thanks
-Chad

harrytm · Feb 25, 2005

Oh, Is this machine a lathe?

harrytm · Feb 25, 2005

I'm talking about tool offsets,the amount the machine "stays away" or "digs in" or varies from the toolpath. Do you have G41 or G42 in your g-code?

GisMo · Feb 25, 2005

Its a vertical mill. Yea we're running tool offsets. But running no offets would require a seperate program for each tool change. Don't know if I have g41 or 42. I don't run the g and m post. But i can try that post and see what happens.

Jim Bass · Feb 25, 2005

Version 6 & 7 of FeatureMill have problems with cutter comp. The program looks OK when you run it on the computer, but when you run it on mill the tool takes some weird paths. I have found that if I remove all cutter comp from the tool offsets in the machine control then the program runs perfect.

Yours, Jim

mochinist · Feb 26, 2005

I bet you have both part line program and cutter comp checked in the program. If you do uncheck part line program and leave cutter comp checked. Tell the program what size cutter you are using and tell the machine that the cutter dia is .0000 . If you need to adjust the size of the part enter a negative or positive value as needed to make the part bigger or smaller. One of the machines I run featurcam on is a centroid control and I had the same problem a few years back. Now that I got it set up I have 100 percent faith in the program running the way it was simulated in featurecam. If there are ever screwups I can always trace it back to a progamming error(me) or the operator's set-up. Good luck.

jdfowl · Feb 26, 2005

Sorry to GisMo for butting into his topic, but I'm currently working with him on this problem in our shop.

The file was originally set to no cutter comp, which locks out part line program. The random circles were created in the tool path with the file set this way. I changed to cutter comp but left part line prog unchecked, and got the same random circles when the m code was drawn with the cnc. I'll mess around a little more with some of those options.

3t3d · Feb 26, 2005

What I suspect is happening is that the CAD is generating very short arc segments. If an arc segment is short enough to be under the tolerance for a move, it either gets output, or interpreted as an arc of zero movement. This is interpreted by many controls as a full arc. The Post is not smart enough to discard arcs that are too short, or convert them to short line segments.
Now, this is just speculation on my part, It has been a problem for other software packages.
You could try to output more digits of precision, say four or five digits. This will reduce the possibility that roundoff of locatins will appear to be a zero distance arc.
Having cutter comp on or off may be a red herring. It may be that one way or another is creating very short arcs. Find a spot with an extra circle, and examine the tool path if possible to see if it did generate a short arc segment at that location.
Assuming I understand what the complaint is.
Pete

jdfowl · Feb 26, 2005

That sounds like a possibility 3t3d. The segment that is causing these full circles was drawn as a polyline in CAD, and is made up of many arcs. I'll look more into this tomorrow.

As far as I can find, precision can only be adjusted in the dialogue boxes in FeatureCAM, all calculations are "double precision arithmetic." I may have to do some tweaks in the CAD model.

3t3d · Feb 26, 2005

I don't know if you can adjust how many digits of precision are sent to the machining center.
I increased the number of digits output to 5
N200 G01 X ##.##### Y ##.##### Z ##.#####

This, along with a software upgrade eliminated the problem for me.
The fact that FeatureCam carries double precision implies that it might carry very short arc segments along, and they are not discarded or converted to short line segments, the POST then fails to fix them, and depending on the number of digits output to the machine, with rounding strategies, they can suddenly become an arc (G02 or G03) without any displacement.

Too bad I'm not a code writer, this is how I propose to fix it.....
My line of thinking is that a POST never outputs any arc gerater than 180 degrees. Anything more is converted to two arcs. This eliminates any full arc appearing to be a short distance arc. After that processing, any arc shorter than a threshold could be converted to a line segment.

Pete

mochinist · Feb 26, 2005

Have you tried FeatureCam tech support, I have used them numerous times and have always found them helpful. About two months ago I programmed a part and for whatever reason whenever I tried to simulate the part being cut it would crash the program. I emailed the file to FeatureCam and they sent me a new version that arrived the next day. I reloaded my program that had been crashing and it ran fine. If you pay for the tech support use it no matter how silly the question might seem, it is much sillier to waste company time try to figure it out yourself when the support has already been paid for.

jdfowl · Feb 26, 2005

Thanks a lot for the help guys.

I changed the part slightly, mostly increasing some of the radii, and the machine liked that.

Josh

cnc-it · Jun 28, 2005

Hi,
Is it possible to change the number of digits after the decimal place on Featurecam when outputting code for angular and feed on 4th axis wrapping? I had this problem at my last job where the fanuc 6mb control would only accept coordinates upto 3 decimal places so threw an error when the Featurecam sent it 4 decimal places. Never did work it out.... :confused:

andrewmawson · Nov 4, 2005

Yes you can change the format of the output by going into the post processor 'edit' (Manufacturing -> Post Process -> Edit) then if you pick up the 'CNC-Info' tab, select 'words-1' and the format of the various output variables can be set - there are several pages of 'words-n' to play with

Search

Largest Manufacturing Technology Community on the Web

Search

FeatureCAM code problems

GisMo

Hot Rolled

harrytm

Cast Iron

GisMo

Hot Rolled

harrytm

Cast Iron

harrytm

Cast Iron

GisMo

Hot Rolled

Jim Bass

Plastic

mochinist

Aluminum

jdfowl

Plastic

3t3d

Diamond

jdfowl

Plastic

3t3d

Diamond

mochinist

Aluminum

jdfowl

Plastic

cnc-it

Plastic

andrewmawson

Hot Rolled

Similar threads