[kawman]

if someone can look at this file and give me some suggestions, on how not to get any cutter marks at the bottom of the part, you can see them in simulation, i have tried adjusting speed and feed, but it seemed to just do it somewhere else, any advise would be much appreciated, the material is delrin

[Claude Boudreau]

if someone can look at this file and give me some suggestions, on how not to get any cutter marks at the bottom of the part, you can see them in simulation, i have tried adjusting speed and feed, but it seemed to just do it somewhere else, any advise would be much appreciated, the material is delrin

forgot to post the file kawman?...

[kawman]

DOH! sorry guys

[jrmach]

Your going to have to send something with a different file ext.A zipped file of a .bbcd file would be best.

[kawman]

sorry we use winrar, cause it opens all types of files .zip.rar.iso and so on, and its free, thanks anyways i guess

[SBC Cycle]

Your going to have to send something with a different file ext.A zipped file of a .bbcd file would be best.

Here's a zip file jrmach.

[SBC Cycle]

if someone can look at this file and give me some suggestions, on how not to get any cutter marks at the bottom of the part, you can see them in simulation, i have tried adjusting speed and feed, but it seemed to just do it somewhere else, any advise would be much appreciated, the material is delrin

One suggestion I have (if you drew this yourself) is to keep a copy of the solid without holes. You will have a lot less code and a much better looking part if you run the 3D toolpath off of a simpler solid.

I can't explain the toolpath. It's either the surface or BobCAD. On my experience with the Equidistant toolpath I would say it's BobCAD. I've had the same results on much simpler surfaces then the ones you are dealing with here. However, I tried to unstitch your solid into surfaces and I get a warning that "At least one face could not succesfully be unstitched". I've received a lot of files like that from Autodesk Inventor and the toolpath has always tried to gouge the part somewhere. If I looked hard enough, I could sometimes find the errant surface but other times I just had to live with it. That problem went away when our customer went to SolidWorks.

Just FYI. I'm stumped.

EDIT: Picture - There's at least one missing surface. That whole area looks like it could use some work. To the right of that corner there is a little piece of triangle that looks like it could also be a problem.

[kawman]

Thank you!! I also said it had to be bobcam, 1500 verses 20k for other software, I didn't create the model, it did come from inventor, which we get a lot of, and I constanly have problems with them, thanks a lot for your input, I'm the only machinist at a fab shop, so they think I can magicly fixe these little quirks in the toolpaths

[jrmach]

Z level rough and Z level finish will work better here,I think..However I am having problems picking the geometry the way I want.We need the Burr?

[kawman]

i gave z-level finish a try and it didnt really give the results i wanted, i also tried planar slice, which at first seemed fine, i ran the sim and right at the end it took a chunk out of the block, im thinking its prolly something to do with inventor maybe something on the surface, what step over do you usually use? this was .015 maybe i should try .002 step, i agree burrman usually has the answer!

[jrmach]

If I try selecting the surfaces one at a time for geometry,if I pick the one shown not selected in pic,it will also select the the side of part.Missing surface there.And I am with SBC there appears to be numerous areas of rework needed.

[kawman]

95% of the solids I get are from inventor, and who knows what was used to draw the original, I do have small problems, usually I can work around them, I have asked for models to be fixed before, and usually they just save in a diffrent format and send it back, what do you guys do when you have problems like this? These jobs don't really allow me to redraw all the models, we do have transmagic which is supposed to be able to repair files, but no one really knows how to use it! could it be bobcad?

[jrmach]

We need a Burr

[BurrMan]

regarding the geometry:

I dont think it's a modeling error. but I'm not so sure it's a BobCad error. If you open the model in an autodesk product, the bad trims are not there. Other apps produce the bad trims. I think it would turn into a he said/she said if you try to track it down. I would have to sit with the CAD guy to know whether he is making bad decisions and Inventor covers his tracks, or if Autodesk is just doing something that alot of other apps arent handeling well... Anyway.......

Machining:

Here's the solid back with repairs that will allow BobCad to work with it (Bad trims removed) I also included one that is slanted at the 5 degree angle. I also used sbc's advice and removed the holes so the toolpath doesnt do anything funny around them.

I dont think equal distance is a good path for this. I think it needs to be broken into 2 seperate paths. The paths wont like to go from vertical to flat, or flat to vertical on a doubly curved surface. This is where the transition marks come in. There is also a slope to the part that will make it more difficult.

"I'm not a machinist, so i have just a suggestion to discuss. I would think that you would want to block the part at the 5 degree angle to remove the slope, then do the part in 2 seperate areas, like a "z level finish" for the top, and a slice planar for the bottom, using boundries to constrain the toolpath.

Splitting the part to these areas or something:



Anyway, maybe with a model that you can work with, some of the others can generate a clean path on it.....

[jrmach]

need a Burr

have I just been Spam Mocked,ha

[BurrMan]

So here's the part with 2 toolpaths to look at. I left the default adv-rough, but am just paying attention to the slice planar and z-level finish to clean the inner area. The other surfaces can be looked at later.

I am looking at the transition point of the slice planar with the z-level finish. I'm not convinced I havnt violated the verticaL wall with the slaice planar yet, maybe someone else can help look.



First, I blocked the part at 5 degree's. I boundried the slice planar at half the diameter of the tool, short of the vertical wall (This should keep the tool from violating the wall. Any closer and the toolpath starts to move vertical, which creates marks with slice planar and large jumps.

The Z-level finish is controlled by a bottom of job setting, to just meet the slice planar. I think there enough room to go down a couple more witches tits, but I dont want to have the finish try to go "Horizontal". The same marks from non-contiguous jumps in the path.

It looks like a good transition. I cant tell from the sim that there is a transition mark. You can just sim this file for the 3 toolpaths to look. Can anybody tell if the slice planar is violating the vertical wall with this path?

[jrmach]

I slowed way down and watched in Preditor,is good for what i can see.Have not played with adaptive rough much.but it appears if the feeds were varied that some of that tool path looks like trochordial milling.Maybe next version,cool.Here is a Preditor look.

[aldepoalo]

I've been following this thread over the last few weeks...

1) When you say you are having tool marks it's un clear to me where you are having them. So could you post a picture of a cut part with the tool marks that are in question.

2) It was a good point to have a model with and with out holes. I completely agree with this concept as not having the holes allows the tool to cut across area's vs going down into them. You can "cap" the holes as well if you didn't want to have 2 models.

3) Sometime you get bad models due to the way the part was designed. Using un stitching and stitching will help you find the problem area. You may need to recreate surfaces from time to time. ( will all systems ) You would think all CAD designers are great at their job, but sometimes they " fudge" things to make them work and it can cause problems with the file when it comes time to machine it. Other times it's just how the CAD system stores the information which BobCAD may or may not like.

4) Surface normals, even through we treat surfaces as solids that have no thickness, the surface normal can play a role the quality of tool path. Not in all cases but it is recommend to have the surface normals facing the same direction ( either in or out). Sometimes a finish quality issue can be based on surface normals not facing the same direction.

5) Equi distant offset is a catch all tool path. This offset tyle will give a consistent surface finish over multiple surface bodies. Where you can run into an issue is with the change of direction. When cutting metals having a change in direction of the tool path can effect the surface finish. So sometimes using a planner tool path to limit the change in direction is all you need to get a good finish. In your example your cutting delrin, which is a plastic right? That being the case I can't see the change in direction having a big impact on the surface finish.

6) Remember if you are going to create multiple boundaries for cutting in 3D, that you always select the whole body or all the surfaces. BobCAD's gouge protection is based on what bodies are selected. So just make sure to select them all and limit cutting with a boundary.

I think burr and others have done a great job expressing concepts for cutting this part. In order for me to help more I need to "see" where the tool marks are on the part to understand what further steps I would recommend to handle them.

BTW I like rar files too

[SBC Cycle]

This image is a screenshot of the Equidistant toolpath, which I believe contains the tool marks OP is referring to.



Here is a screenshot of a Slice Planar toolpath I created on the same part, same stepover.



The slice is a lot cleaner at the same relative angle. Even if I choose a slice pattern angle that doesn't allow the tool to cut "cleanly" across the part (like a 45 degree angle), it's still smoother than the Equidistant in this area. Is it the surface or the toolpath?

[kawman]

Thanks, Al, Burrman and everyone that gave me some advise, i would show the gouges but the part has already shipped, i also just think it had to do with change in direction, i guess i was being kinda lazy just using equidistant offset, thanks again guys, this gives me alot of information to work with when im trying to plan a job,