[flatform]

Hello there folks,

Have read many informative posts here and would like to thank you all for sharing stuff!

I am trying to setup and use a Haas TM2 with the 4th axis option, no tool changer and RS232 communication. I have a hefty background in IT, design, CAD, small constructions and desktop laser cutting machines yet I form a complete newbie in CNC milling, THUS facing problems using SolidCAM and the TM2 in general. Somewhat gathered, my questions are:

1a. Do i HAVE to define a new machine identical to our TM2 including dimensions and all parametres (i have created the STL model and imported correctly dimensions/axes in .vmid file) AND write a pre/post processor for it... so that we can safely use the g-code? The .vmid machine is it just for simulation but pre and post processors must contain all accurate data (Hp, speeds, table length)?

1b. SolidCAM offers the following options: gMilling_Haas_3x, gMilling_HaasSS_3x, Fanuc, g_milling_3X, g_milling_3XB, g_milling_3XDC

G-code output with Haas options gives BAD NUMBER error when sent to the machine, Fanuc option works bad -my local Haas dealer later suggested it and US support told me to avoid it due to differences in canned cycles- and resulted in a spooky error while on a test drilling cycle (tool forgot to raise and went through the part -foam-) Will it be safer not to use such cycles till i find an 100% compatible post processor?

1c. In case i really need a post processor to mill with safety, is there any company that i could get one from or anyone here with experience on the field? (writing one myself could be possible with some help but maybe better not in this moment)

2. When i install and start using the 4th axis, is an addition of it's properties in both CAM's .vmid and pre/post processors enough for it to export correct g-code? (still wonder how i do that Any hints on 4-axis programming/coordinates will be welcome.

Will demo TopSolid 7 as well, to see Haas implementation there, anyone having experience with that CAM? (TopSolid's 7 CAM part is the first PCAD i used, very intuitive and not error-prone like SW i.m.o.)

I have been so discouraged by canned cycles errors described above and cannot wait to get into actual machining, with great precautions but no fear

(working on foam for starters helps

[glovebox20]

It will be safer for you not to run your machine until you can read this:

%
O00010 (drill test)
G0 G28 G91 Z0
T1 M6
G0 G54 G90 X1. Y-1. S1000 M3
G43 H1 Z1. M8
G83 G98 X1. Y-1. Z-.56 R.05 Q.22 F6.2
X2.
G80 Z1. M9
G0 G28 G91 Z0
G28 Y0
M5
M30
%

Anyone who cannot read this should not be allowed to program/setup a cnc mills for their own saftey in my book. Even better if they can write it.

Canned cycles sure makes programing holes lot easier vs a bunch g moves.... just wait until you start to milling with cutter comp. Your head will probaly hurt for a week until you figure it out. I know mine did.

With that being said, all you need is a post for machine to genrate g-code. All the other stuff is just bling. Nice to have, but not nessacary. The gMilling_Haas_3x is proably the closest post you have that you need. You will have to mod the tool change cycle to handle manual tool changes. I'm sure you will find a few other things as you go along. A lot easir to know what post you need (or how to fix it) once you know how to read AND write g-code.

[flatform]

glovebox20, thanks for your immediate reply

You are absolutely right about g-code knowledge and safety, and that is what i have been doing these days, and why i mill only on foam...

Checked the g-code output and the drilling operation started with a weird G98 G0 !!!! -25 etc, a post-processor error(?)?

Then while fiddling around with an option (just a tick) to shorten the code or not in SolidCAM, the problem disappeared and never got back, I was not able to recreate the G0 output which felt like a SolidCAM bug (which is even worse).

The drilling operation was still a mess even though i triple checked the tool offsets in the TM2, furthermore after G0 disappeared a M29 option appeared that was unrecognizable by the TM2. Tried with making holes one by one and still, will try more tomorrow. Since the target is to be able to produce, clean g-code from the CAM, i must find a way to correct the post processor right?

I was really concerned about the post-processor and now even for program bugs, will get back to the TM2 tomorrow and read again the new code to try to run into some temp conclusions and post them precisely here. I am thinking about the TM2 coordinate system setting which is now Fanuc, i read from the manual it affects only G92/G50 codes, not appearing in this g-code output.

I will try TopSolid CAM -while reading more g-code- to see how the post processors work there.

As for cutter compensation -i guess i will need it quite a bit later...- i cannot really understand the issues now. Do you mean i shouldn't use cycles even for drilling?

I would be great if you can propose me links with free training material, e-books, well structured advises/workflows etc., for new cnc users.

Thanks again

[glovebox20]

Hello

I would say your top priority should be learning the G-code cause that will make everything else easier to do on the mill. Then worry about the cam system. Knowing the code will make using the Cam system easier to use because you will know what kind of code you’ll need to use to achieve your desired results, and it makes debugging your post much easier if you know what code you are looking for.

How are you handling your manual tool change? I posted a standard Haas VF post you can try. If you want the tool change modified, I may be able to help you out. I use Inventorcam so our cam files won’t be compatible. There Should be no G0 in the Canned cycle line (G74,G81,G82,G83,G84,G85, etc.) . G0 will cancel your canned cycles (like G80) in most Fanuc, Haas machines. The G98 brings the tool to the ‘initial level’ before it moves to the next hole in a canned cycle. G99 will only bring your tool up to the ‘R’ level before moving to your next level. Which is fine if there is not clamps in the way and your R plane is above your work surface. I attached a notepad file showing you the differance between the two. Should work on your HAAS Mill. Dimentions in metric.

[flatform]

hello back,

i had no time today to work on the machine, hopefully will test your attachments tomorrow, can't wait to be honest.

Got the Solidcam files though and here are the Drill Settings Screenshots in Solidcam and the output code (last two drills are a test for 0 drilling, stupid test yes) belonging to the Part_2-1_drill_sep.NC

Unfortunately i do not have the other g-codes operation settings in Solidcam, they where overwritten. If i remember properly it was a drill recognition operation with Auto find holes which resulted in two groups. One group was only the central lower level hole. Drill type was G83 with only the Step Down data entered (i think 5). I have included the D_drill_2 files which were just compiled in my home pc. I feel embarrassed not to have understood yet when the N line numbers appear or not. I am not sure whether i get a bad number error from the TM2 when they do, oh my, trying to learn fast generates inconsistencies but what can i do, it must be done.

All my tools where zeroed based on T1, which has 0 length entered in TM2 and was used for G54 part zeroing as well. All milling operations (pockets, profiles, 3D, etc) worked fine with my setup. What the drilling does is that it jumps to Z -25 in rapid and then just rapids on the same level making no drilling, or something similar, must check it again but i guess it does what the code says... the r1.NC gives that weird M29 S1000 special command, not understandable by the machine (cycle stops and we get error alert something like command uknown). Always remember my feeds are for foam, and we work from manual 30% feed and up while testing, they are safe.

(was weird that the Haas guy who came some years ago to setup the machine -which was left abandoned up to now that i came to help my friends use it- left relative tool zeroing instructions and absolute parameter in the TM2... we almost had a HUGE crash because of that)

Another thing, the same guy left scaling to default, which resulted in all parts (we dry run) to be miniaturised, maybe 1000 times smaller, i changed that to integer and everything works as expected. I guess that is a matter of the Post processor as well, to format the numbers with dots (ex. 10. for 10mm, 10 for .010 mm) ?

And one last, quite simple yet annoying and i haven't found it in the manual yet for some strange reason: When i enter data, tool number, offsets etc. the number i type adds to the total, and must enter it in 12. format to be mm. How can i force the data to overwrite? otherwise i must subtract the amount in both mm and mm/1000 first to zero then and then enter the desired values. An easier way?

Thank you for your time once more, that is what i do too -actually most of my day usually- in the various fields i know very well and i feel confident i can help.

[glovebox20]

When setting offsets, write/enter will add the value to your offset. F1 will set the offset with the value you have entered. The easiest way to touch tools off is right off your part using the tool measure button by the F keys. This way your Z workoffset is zero. They are other ways to achive this as you get more fimlar with CNC's.

M29 is typlical used for tapping on a Fanuc control. It times the spindle with the Z axis for ridig tapping. Something you shouldn't have to worry about on the Haas control.

Sounds like the person who ran the machine before you had some odd habits. I guess we all have our own ways of doing stuff. I personanly don't like useing drill reconition with Solidcam, but that is just me.

I'll look at your .rar files when I am on a real computer.

[flatform]

hello again,

Gathering all debugging i end up here:

1. Bad Number errors in Haas TM2 using SolidCAM and all processors other than gmilling_Haas_3x, when using metric system must be due to the use of 4 and not 3 decimal numbers.
The Haas_VF post processor you kindly uploaded has the same problem, i must manually edit it using instructions from this post: http://www.cnczone.com/forums/solidc...lways_3_a.html although this post is rather old and .cam files mentioned are maybe now .camdbx files, not accompanying n every machine.

2. Even with the Haas_VF post processor you provided G83 cycles are maybe not correctly implemented, g-gode output for a G83 stepped drilling come out as:
G98 G83 X14.6252 Y-52.1702 Z-20. R2. Q0. F500. where is the step down factor (5mm)? I think i should not use the use cycle option as you suggested, to many errors lost in translation unless i write the post-processor myself with caution. Wish i had the time to play around with that.

3. gmilling_Haas_3x G83 step drilling produces DISASTROUS code, we should avoid it in all cases, unless we uncheck the "use cycle" or "minimize hole cycle" options (which produces long, basic G00-G01 up/down drilling, no true G83). If not, a G0 rapids the spindle in the desired hole level, more than that, it does not raise above part level and rapids through the part to find next hole!! So surprised such an expensive program to have this "alpha like" -not even beta- version bugs. It is just a bunch of post processors solidcam offers/have to maintain and it is a disgrace they cannot do it properly. Wonder if i was not demoing it and had actually paid for it. How could one trust such a release without checking every single line of the g-code for absurd translation or running it in single block mode every time a new function is used??

4. Is there someone in this forum that could write/alter a post processor for solidcam? on a free or paid basis.

At least with all the errors i was forced to learn proper G-code to the level i can debug simple stuff, which is what you suggested from the start...

Thank you for your help up to here!

[glovebox20]

The Haas_VF post I sent you was a gmilling_Haas_3x to start with. I only used it in inch mode.

If you have a problems with the code, could you post it. It will help to debug these problems. I attached a 'drill test' screen shot. I just want to make sure you are entering a value for 'Q' in the 'Drill Options' (press the 'DATA' button under drill type to open window).

I can provide some assitance to mod your post. I'll help you out with the Drill cycles and Tool changes. I'm using Inventorcam 2012, so there may be a translation error there, but we should be able to get something to work. At least make it so it do crash your machine.

Not saying there post are perfect, but I haven't had too much trouble with the drill cycles. There was a error with the tap feedrates wich took me 8 months to find. Soildcam tec. support was not much help finding this bug, but it dosen't hurt to give them a call.

If you have more qustions with Solidcam's post, maybe you sould post them under the Solidcam fourm.

I've used Gibbs Cam, Bob Cad, and Solidcam, PC Max (Hurco), CIMCO Edit V5, and tested OneCNC for Fanuc, Haas and Fadal mills and all there 'standard post' sucks. I dout any other CAM system would be different. Once we get a post figured out for you, it souldn't be too much work to keep it updated, unless you want to add more features to the post.

[flatform]

hello back,

i attach the screenshots, are they ok so you can see what is wrong?

(images were resized from server if you find them difficult to read i will re-upload)

if the gmilling_3x G81/G83 cycle is correct, then i can try to copy/paste the correct post processor part to the gmilling_Haas_3x post processor, or use the first in all my parts.

I haven't really understand what is the Q value, when i leave it 0 and change only the Step Down value, ie. 5mm, when running the simulation i see something logical, the drill advances 5mm at a time, when using Q only the drilling goes down in one step. Another thing is that with the options you see i get a crash warning on each hole, in appx. the middle of each depth, while running at Z with feed rate not rapid, present in al the holes except the last one, in both 3x and Haas_3x, any clue??

Another thing, the parts i have to machine must be done using our 4th-axis. the have millings in all sides and the stock is round. I did them using multiple fixings yet it is time concuming and introduces time-consuming zeroing procedures and i have to be really precise. Should i use the Mill-Turn module in Solidcam? Or could i just inject some Y axis rotation in the code? I have only two post processors available there. I shall post this in the Solidcam forums you are right.

thanks for your time once more!

[Machineit]

I haven't really understand what is the Q value, when i leave it 0 and change only the Step Down value, ie. 5mm, when running the simulation i see something logical, the drill advances 5mm at a time, when using Q only the drilling goes down in one step. Another thing is that with the options you see i get a crash warning on each hole, in appx. the middle of each depth, while running at Z with feed rate not rapid, present in al the holes except the last one, in both 3x and Haas_3x, any clue??

"Q" is the peck or increment amount in Haas canned drilling or milling cycles. It is how much the drill goes down with each peck or the step over amount in milling cycles like G13.

It is fine to let your CAD system write complicated code, but you REALLY need to understand your basic cycles and G-Codes. You should be able to know what each line of code is going to do or you will find yourself in big trouble.

If you are just starting, writing a circle or radius move, for a corner say, is fairly intimidating, but writing a simple drilling cycle is pretty damn easy. If the software is asking for the "Q" value and you have no idea what that is, you will soon have issues.

Study your manual and learn the basic G and M codes. Canned cycles like G81, G83, G84, G85, G12, G13-----Learn what they are. In learning them, you will learn the other codes of the canned cycles like--- Q, R, F, L, I, K, etc.

If you fully depend on your CAD/CAM system and don't know basic code you also can't understand your CAD software.

Not to put you down, but if you can't write a simple G83 drilling cycle, then you need to stop with the CAD and go to your machines manual.

Good learning.

Mike

[flatform]

Machineit, thank you for your answer.

The point is not me understanding the gode, -which i do at the extent i have studied it- and that is why i compare it to what i see in the SolidCAM simulation. I can now write a simple G83 drilling by hand on the machine and run it, but a software that i am willing to pay thousands of euros to buy and use CANNOT, and that what makes me totally frustrated, because in SolidCAM simulation that works only when i put a number in Step Down, it just ignores Q and continues outputting wrong g-code in an inconsistent way described in the end of this reply. Is there any connection of what i see to what i will get or not?

Of course i should -almost- blindly trust my software, that is why we pay for it and that is what post processors are for, otherwise i would write it all by hand and waste all the IT tools.

In any case, should i be prepared for this:

G98 G0 Z-20. R2. F500
instead of
G98 G83 Z-20. Q2. R2 F500

when i say to the CAM drill me a G83 hole? not even the G83 is there, skip that whatever G0, skip that the code following does not lift the drill and goes through the part to find the next hole... What about a 5 or more axis post processors? Should we trust them or not? Because even the most experienced machinist would need days to check every line of code for a complex part!!

Plus, there are numerous, if not most of the CNC users i know that do not know G-Code at all, somebody has setup a proper workflow for them and they follow it blindly with no accidents. That will not be my case -i want to learn it in total- but may be the case for the people i leave behind to work on the machine, it is their machine and they are not code freaks in any case...

I totally support learning g-code, for safety reasons and handy reasons. I can even combine it with grasshoper in Rhino and make a small CAM software myself, but this must not the case as i understand it, when you buy a CAM software.

Modifying a post processor to add some capabilities (special M functions or whatever- that a specific machine has is logical. Critical errors in standard format g-code are not acceptable, in a Release Version (not beta).

One thing i know is that on my first day on the machine i was able to mill on foam a complex part with finish passes, and the only thing that went wrong where the drillings, possibly due to a buggy post processor, if that is the case and not my ignorance.

Read if you can spare more time my previous post/screenshots again and you will see my problems, Is it SolidCAM that produces disastrous code when i have the "use cycle selected" and Haas_3x post, or me? When i use the gmilling_3x post, i get what seems to be a correct code but will not show correct when simulating, that is the frustration i get!

What makes me even more disorientated -i just hope it is me doing the wrong
things, that would be a relief- is the fact that i am having trouble recreating my issues. I work one two machines i personally installed windows 7 + solidworks + solidCAM following the exact same procedures -definitely- and drilling tests procedures (from creating a new part to starting a cam) i haven't narrowed when SolidCAM/post processor (even on the same machine):

1. PostP Produces wrong G83 code using cycles (corrected by restoring the original .vmid file in Gpptool directory, from a backup file present in the same location, the original machine file was somehow altered)
2. PostP Gives me dimensions with 4 decimals (1.0000) and not 3 decimals that my machine can read and gives BAD NUMBER error (machine is in metric) > (corrected it in my home pc by modifying .gpp files: numeric_def_f, xpos_f, ypos_f, zpos_f = 5.3, will check work pc)
3. PostP adds N numbers in each code line. (corrected in my home pc by modifying .gpp file: bulknum_gen = false, will check on work pc)

If i am doing something "strange" is that when checking for correct drilling cycle code, i change my machine form the CAM-part definition, without creating a new part. When changing to Fanuc i think i am forced to create my drillings again.

Any clues at least for the decimal inconsistency??

It is easy to blame me, i hope it is me, but if it is not, what could it be?
(rhetorical questions)

thanks again mike,

constantin

[flatform]

By the way, i am using SolidCAM X64 2012 SP1 in Solidworks 2012 Premium X64 SP4, on Windows 7 Home Premium X64.

[glovebox20]

flatform, I completly understand your frustion with your post processors. far as 4x or 5x post gose, yes you can trust them, as long you test them out and know what settings to use in your cam software to get the results you want. All part of learning. Your cam system is only as good as your post, so if the post is is great......

What post do you have the most luck with? It may be time to pick one and start modifing from there, Unless your can find another post to use. I like the D_drill2_gmilling_Haas_3x_use cycle from your .rar upload earlier, but I'll let you decide what works best for you.

If you mod your post to out put the correct deciamls and N number, I say you have a good start of understanding how your post works.

You just might find out that it's easier to program your 4 or 5 axis drilling by hand than using your cam system. Some poeple cam out the part, then add the 4th axis moves them selfves.

I would say your problems are coming from not knowing the code, not knowing your cam system, and post processor errors. But I seems like you are heading in the right direction. Keep ip the good work.

Why don't cam systems come with better Post? I think it might be to reduce poeple from copying there software illegaly, or their post writers don't know how to write G-code them selfves.

[glovebox20]

If yoour graphis are crashing, you might want to check your stock size, make sure it's not bigger than what you think. When your create a new Cam Part, there is a Cam setting (stock definition) that controls how much oversize to make your stock in each direction. Might want to look at that. Also, make sure your 'upper level' in your opeertion is above your work surface, or you might run into problems.

Yes, you may have to redo your Drill operation if you change your machine type, depending on your drill/coolant options you have advablie for each machine.

[Machineit]

By the way, i am using SolidCAM X64 2012 SP1 in Solidworks 2012 Premium X64 SP4, on Windows 7 Home Premium X64.

Again, I did not mean to attack or hurt you, but you are posting in a Haas forum not a Solidworks forum. There is a Solidworks forum you know.

You say it is 2012 software, so can't you contact them for assistance. If not, I would post in the Solidworks forum and ask them for help. There are many more Haas users than Solidworks users, but you will have more luck finding software help in that forum.

I did look at your pictures, but they are very difficult to read or see. In the third image there is a "Q" call out in the post in the drilling cycle. Does that not work with your machine? If not, what does it do?

I am just trying to help.

Mike

[flatform]

hello mike,

no worries, it is frustration from my side not defense! i started in this forum because i did not know whether it was my fault, a haas TM2 setting fault, or solidCAM's fault. Learning fast has inherit problems...

I will check whether fore some strange reason my two solidcam installations/post processors have differences that produce such inconsistencies and move remaining solidCAM questions in the appropriate forum, as mentioned in previous posts.

Pics where resized automatically i should post screenshots les than 1000px next time! They can be read a bit better by using ctrl+ to magnify browser contents.

I am sure i will have more Haas related questions and will be glad to receive any future replies.

thanks again mike, keep on machineit-ing.

[flatform]

glovebox20,

As you suggested, I had no other option from learning some g-code and some of how my post works. At least to debug basic stuff.

For the little part i have to prepare in the next days, i think i will go by injecting some A axis rotating code by hand or even from the TM2 manually, it is just 3 or 4x 90 degree rotations/positions anyway.

I guess i will have to use a code for the program to pause -will check which code- and wait till i rotate the A axis and push the cycle start to continue, or find which code rotates my A axis and use that, something like let's say G00 G91 A90 or A-90 when i want opposite incremental rotation? Is there absolute rotation? I should read on that. Could i Home/Zero my Z axis to a certain degree each time? (let's say for working with rectangular parts, so i don't have to level the part each time)

The post at work will be modified as well and check for inconsistencies there.

Once the post produces the same errors for the same moves, i will be more able to debug it in a sane manner...

I think my Post does not translate the Stepdown Data Value (G83 type) to a Q value when outputting the code, it should be added. Otherwise i get Simulation that shows the Peck (ie. 5) but the g-code has peck Q0. What i would do for now is enter the same values for Q and Step down, to get both, till i mod the post.

The simulation crash is strange, as it occurs in the middle of the Z level, while feeding the drill down. The cutting length is bigger than the hole. The stock is always created in solidworks, usually for the test it is 5mm bigger on all sides. I will triple check my upper level number, when you say work surface you mean the surface about to be operated (drilled, faced, etc) and not the part or stock upper level i guess. I set the upper level to be exactly on the surface i am about to ie. drill, by choosing it graphically. Should i put there a delta value to get it ie. 2mm higher?

Thanks for your suggestions, again.

[glovebox20]

glovebox20,

The simulation crash is strange, as it occurs in the middle of the Z level, while feeding the drill down. The cutting length is bigger than the hole. The stock is always created in solidworks, usually for the test it is 5mm bigger on all sides. I will triple check my upper level number, when you say work surface you mean the surface about to be operated (drilled, faced, etc) and not the part or stock upper level i guess. I set the upper level to be exactly on the surface i am about to ie. drill, by choosing it graphically. Should i put there a delta value to get it ie. 2mm higher?

Thanks for your suggestions, again.

Correct,but if your stock is 5mm oversize on all sides, your upper level should be 5mm insted (top of stock), not top of your part. You can cheat this by adding a larger safty value, but not recomended. Better to change your stock def. to match your part. By work surface, I mean the surface your working on. So if your stock is 5mm oversized, your work surface is 5mm above your part. Unless you face the extra material down in a preavious OP.

What do you mean by step down for drilling? I'm only aware of the 'Q' value.

[flatform]

first of all, i would like to say that all my post-p related problems are solved now. decimals and line numbers are ok in both pc's and G-83 drilling cycle looks ok to my eyes, haven't checked on the TM2 or cross-checked the work one with my home pc output as i was in a hurry.

in the work pc, gmilling_Haas_3x.vmid was somehow altered and there was a backup file present. i replaced with the correct one and it is ok. This is not a default SolidCAM post-p error then, 99.9%. Good thing...

the Step down value is referred as a Peck value in SolidCAM manual, is present in the same "Data" popup in a G83 cycle, something like a Q value, and it is only used in the internal Machine Simulation in SolidCAM and does not affect the Q value in the g-code output, in my tests at least, no additional information in the manual. It is very weird, because in order to have an accurate machine simulation (or solid verify sim etc.) you need to enter this value to be the same as your Q value. I haven't tested if the simulation listens tou IKJ programming, very very strange. That is what caused my frustration, because i followed SolidCAM's manual instructions and entered the Step down Value instead of the Q value i was reading in the Haas Manual...

I guess before i leave Rodos Island (far from the capital, difficult and expensive to get training technician here...that is why i am doing it)the post-p should be modified to output the Step Down Value as a Q Value and remove all the other options by modifying the Pre-p, to make it simpler for the people who will use it. Otherwise they should remember to put the same Value for Q and Step Down, which is not so bad, to get a proper simulation. At least that is what occurring to me now.

I would like to thank you all for your suggestions, one way or the other they guide to a walk-able path, but thank you more for your understanding, precious for a newbie...

will write about the levels on my next post.

[Machineit]

glovebox20,


For the little part i have to prepare in the next days, i think i will go by injecting some A axis rotating code by hand or even from the TM2 manually, it is just 3 or 4x 90 degree rotations/positions anyway.

I guess i will have to use a code for the program to pause -will check which code- and wait till i rotate the A axis and push the cycle start to continue, or find which code rotates my A axis and use that, something like let's say G00 G91 A90 or A-90 when i want opposite incremental rotation? Is there absolute rotation? I should read on that. Could i Home/Zero my Z axis to a certain degree each time? (let's say for working with rectangular parts, so i don't have to level the part each time)

You can use Absolute or Incremental with the 4th axis. In Absolute drilling four equal holes would be for example is G00 G90 A0., A90., A180. and A270. In Incremental i would be G00 G90 A0., G91 A90., A90. A90.

Don't forget the decimal points, ".", and don't forget to go back to Absolute G90 mode at the end.

Best of luck---tough times everywhere, but you guys are getting hit hard over there.

Mike