Fusion 360 - WCS Location Options
ฝัง
- เผยแพร่เมื่อ 28 ก.ย. 2024
- This video will look at different options for locating the WCS when creating a setup along with the strengths and drawbacks for the different WCS location options.
Have a project you need help on? Contact me at www.mechanicaladvantage.com/schedule-now
1. Operation always middle bottom of parts. I created cnc programs that set G54-G57 coordinates with Z0 resting position of serrated jaws. Mine have 3mm holding height. I model 4mm stock on bottom, 1mm on top. I mill 0,6mm under part, so 0,4mm over jaw. I model extra side stock to be sure adaptive will not break tool when stock is oversize. You will never ever crash mill in jaws this way. If stock is smaller, top of part will not be machined. Thats all. Operator is eyeballing X0Y0 and probe in cycle will set middle of stock for even sides during adaptive.
2. Operation I use always bottom left rear corner. I made several cnc programs with name of parallel heights. When operator needs 45mm parallels (I write him in program) he will just quickly run program which sets G54-G56 for 4 corners of vice and Z0 on 45mm parallels. This way the setup is fast as hell and since then accidents droped almost to zero.
I probe all operations in cycle. Operator is always just eyeballing X0 Y0.
In 2. Operation to probe corner in cycle, I will mill off ,,hat,, around part or just hat in probed corner (this way there is no big burr for probe). I mill it about 0,3 mill over top of part
See my comment for an idea that might work for you. Write a kind of incremental G10 macro and then you can use both. Offset the initial WCS from the fixed point, to a WCS based on the stock. Works well with probing the stock then, yet initial offsets can be be set in CAM. Works across multiple machines even, with vices not in the same location!
Your videos are Always SO good!!!
Thanks Al. I'm glad you think they are of value.
Can you discuss Op2 scenario's hard jaws for rectangular part and Soft jaws for others - how to get WCS to finish part.
I don’t understand the WCS being under the pallet? Can you spend more time on setting tools, etc… in relation to the optional WCS’s?
The idea is that those workholding components are very precisely made. So you can create a digital twin in Fusion. Once you touch the spot off on the plate that I show, that is the WCS for any setup that uses those components. It's a pretty slick system that is used by prototype shops etc. for low volume high mix parts so you can quickly go from job to job.
@@MechanicalAdvantage I’m sure I’ll figure it all out. Thanks.
@@MechanicalAdvantage can comfirm. i use that everyday and just centre the stock with a caliper and hit run.
is also good for simulation and collision avoidance because the WCS never moves.
On 5 axis machines we had to use center of rotation as location of XYZ. The build had to match the setup. Today's 5 axis have a Dynamic work offset G254. You set to center top at A zero B zero and the machine will do the math when it rotates.
Another advantage of basing the Z origin on the work holding is the accuracy of your collision simulation isn't dependent on the exact height of the workpiece so you can cut close and it'll work every time.
Thanks Kevin, another very useful video, thanks for your time to make these for us 👏
I tend to appreciate setting the z portion of the wcs relative to the part or stock (often the top) as it makes it easier for me to look at coordinates in g code and translate that to something in reality (e.g. if I see a z-1.25, I know that means 1.25 inches below the top of the stock.
Hi Gina. I'm curious. Do you watch the numbers on the control as you run the program that closely? My go to method is how I do it with the how to run an unproven program video I did a while back. As long as I know I'm not going to crash into the vise etc. I'm feel pretty good with that check.
Kevin....great video....just getting started with a 770M and was wondering if you know of a technique for doing 3 axis chamfer operation in F360...I've tried the Scallop operation but with very little success..do you know of an alternate approach...?
th-cam.com/video/XaV-KgnQTO8/w-d-xo.html
Love your videos!! Super helpful, informative and intuitive. The question that I have is where did you acquire the model for the Mlock vise. I have looked everywhere and can’t find it… help please
Sorry for the delayed reply. Email me. I can send you the model you have.
I’m experimenting with a half/half process. I have fixed points on the vice as my reference. But the WCS is say underside midpoint of the stock. I then have a macro which is something like an incremental G10, which sets up say G54 based off the reference points. This is done with a manual NC op, and the offsets are measured off the model manually.
I’ve an automated probe on the machine, so I usually then do some automated probing to update the stock position to a few microns,etc. Those who use work stops could just go to the machine, check where the stock is and come back and update the params in the NC code.
I’m generally setting this up as a setup type program to be run once before the main program. Basically to semi automate machine setup. The benefit is that tool Z min is quickly inspected to see if it touches the jaws (eg nothing should go below 2mm for my serrated jaws). However, the program is unchanged if I move the vice and I can tweak the precise WCS by hand if needed.
Disadvantage is the manual step to enter the offsets (measured from within cad). However most users with a small number of vice/jaw locations will be reusing the same params in every program.
I wish such a feature was within fusion to automate the offsetting!
Well I would not set up my coordinate center to a point that will be machined right on the beginning of the process if possible. As if I need to remove the material out of the wise or the machine goes nuts during the work.. like if the machine get stuck in the piece or who knows why which would mess up my coordinates and offsets I would not be able to reposition the piece or machine back. If you work in production of large batch, sure, you can throw away the piece and run another.. but if you design and manufacture piece by piece and things get changed on the way quite a bit it is always handy to keep the center as long as possible.
I found the bottom corners much better as I can also use that point while turning the model upside down. Well not 100% times but 99% more that upper right corners ;)
Bottom corner is not always the best though, sometimes a hole or corner of the model that is reachable from more sides can serve as referential.
Sure upper corners are the easiest to work with on simple parts.